MSC Patran software Reference Manual
Publicité
Publicité
C O N T E N T S
MSC.Patran Reference Manual
Part 6: Results Postprocessing
MSC.Patran Reference Manual,
Part 6: Results Postprocessing
CHAPTER
How this Guide is Organized, 3
Capabilities and Limitations, 13
User-defined Defaults Function, 34
Examples of User-defined Defaults Function, 35
■
Creating and Modifying a Cursor Plot, 124
Create a Cursor Plot of von Mises Stress, 139
■
Create Loads or Boundary Conditions, 235
Overview of the Insight Application, 248
Capabilities and Limitations, 253
❑
Isosurface Coordinate Selection, 265
Isosurface Attributes Form, 267
Cursor Results File Format, 287
Cursor Results File Sorting, 288
Result Case(s) and Definitions, 293
■
Problem 1: Linear Statics, Rigid Frame Analysis, 330
Problem 2: Linear Statics, Cross-Ply Composite Plate Analysis, 335
Problem 3: Linear Statics, Principal Stress and Stress Transformation, 343
Problem 4: Linear Statics, Plane Strain with 2D Solids, 352
Problem 5: Linear Statics, 2D Shells in Spherical Coordinates, 358
Problem 6: Linear Statics, 2D Axisymmetric Solids, 363
Problem 7: Linear Statics, 3D Solids and Cylindrical Coordinate
Problem 8: Linear Statics, Pinned Truss Analysis, 378
Problem 9: Nonlinear Statics, Large Deflection Effects, 383
Problem 10: Linear Statics, Thermal Stress with Solids, 387
Problem 11: Superposition of Linear Static Results, 391
Problem 12: Nonlinear Statics, Post-Buckled Column, 401
Problem 13: Nonlinear Statics, Beams with Gap Elements, 408
Problem 14: Normal Modes, Point Masses and Linear Springs, 411
Problem 15: Normal Modes, Shells and Cylindrical Coordinates, 415
Problem 16: Normal Modes, Pshells and Cylindrical Coordinates, 421
Problem 17: Buckling, shells and Cylindrical Coordinates, 426
Problem 18: Buckling, Flat Plates, 429
Problem 19: Direct Transient Response, Solids and Cylindrical
Problem 20:Modal Transient Response with Guyan Reduction and Bars,
Springs, Concentrated Masses and Rigid Body Elements, 436
Problem 21: Direct Nonlinear Transient, Stress Wave Propagation with 1D
Problem 22: Direct Nonlinear Transient, Impact with 1D, Concentrated
Problem 23: Direct Frequency Response, Eccentric Rotating Mass with
Problem 24: Modal Frequency Response, Enforced Base Motion with Modal
Damping and Rigid Body Elements, 456
Problem 25:Modal Frequency Response, Enforced Base Motion with Modal
Damping and Shell P-Elements, 462
Problem 26: Complex Modes, Direct Method, 465
Problem 27: Steady State Heat Transfer, Multiple Cavity Enclosure
Problem 28: Transient Heat Transfer with Phase Change, 475
Problem 29: Steady State Heat Transfer, 1D Conduction and
Problem 30: Freebody Loads, Pinned Truss Analysis, 482
MSC.Patran Reference Manual, 487
Part 6: Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
1
Introduction to Results
Postprocessing
■
■
■
■
■
■
1
2
PART 6
Results Postprocessing
1.1
Overview
The MSC.Patran Results application gives users control of powerful graphical capabilities to display results quantities in a variety of ways:
•
Deformed structural plots
•
Color banded fringe plots
•
Contour line plots
•
Marker plots (scalars, vectors, tensors)
•
Cursor plots
•
Freebody diagrams
•
Graph (XY) plots
•
Animations of most of these plot types.
The Results application treats all results quantities in a very flexible and general manner. In addition, for maximum flexibility results can be:
•
Sorted
•
Reported
•
Scaled
•
Combined
•
Filtered
•
Derived
•
Deleted
All of these features help give meaningful insight into results interpretation of engineering problems that would otherwise be difficult at best.
The Results application is object oriented, providing postprocessing plots which are created, displayed, and manipulated to obtain rapid insight into the nature of results data. The imaging is intended to provide graphics performance sufficient for real time manipulation. Performance will vary depending on hardware, but consistency of functionality is maintained as much as possible across all supported display devices.
Capabilities for interactive results postprocessing also exist. Advanced visualization capabilities allow creation of many plot types which can be saved, simultaneously plotted, and interactively manipulated with results quantities reported at the click of the mouse button to better understand mechanical behavior. Once defined, the visualization plots remain in the database for immediate access and provide the means for results manipulation and review in a consistent and easy to use manner.
CHAPTER 1
Introduction to Results Postprocessing
3
1.2
How this Guide is Organized
The Guide is broken into the following chapters to provide a logical flow.
An overview of the Results application. It is important that first time
users read this thoroughly to fully understand how the Results application works. Important definitions are defined to understand how results data are stored in the database and how they are manipulated by the Results application. An overview of the operation of the Results application is also provided to give a basic understanding of how to create and modify result plots and how to post/unpost or delete existing plots and results data.
Eighty to ninety percent of all postprocessing needs are accessed through the default Results application form. This chapter explains the Results application default form and how to create quick fringe plots of any scalar data and quick structural static deformation plots and modal style animations and combinations thereof.
Detailed explanations of how to create and modify deformation plots as well as how to change display attributes, target entities and other options.
Detailed explanations of how to create and modify deformation plots as well as how to change display attributes, target entities and other options.
Detailed explanations of how to create and modify contour line plots as well as how to change display attributes, target entities and other options.
Detailed explanations of how to create and modify marker plots
(scalar, vector and tensor plots) as well as how to change display attributes, target entities and other options.
Detailed explanations of how to create and modify cursor plots as well as how to change display attributes, target entities and other options. Also instructions on how to create a report from the cursor plot.
Detailed explanations of how to create and modify graph (XY) plots
(including beam data) as well as how to change display attributes, target entities and other options.
Detailed explanations of how to create and manipulate animations of most plot types as well as how to change display attributes and other options.
Detailed explanations of how to create and display reports of results data as well as how to change report formats and other options.
Detailed explanations of how to derive, combine and scale results data as well as how to select target entities, define transformation, derivations and other options.
1
1
4
PART 6
Results Postprocessing
Explains the capability to graphically display freebody diagrams and create new loads and boundary conditions from MSC.Nastran grid point force balance results.
Detailed explanation of the Insight application (another MSC.Patran postprocessor). This postprocessor has much of the same functionality as the Results application with the exception of results derivations/combinations, reports, graphs, and freebody. However the Insight application allows for some additional advanced postprocessing tools such as isosurface, scalar icon, value, cursor, and streamline plots.
Detailed explanations of the many numerical manipulations that are exercised in the Results application. These include operations such as vector and tensor to scalar calculations, extrapolation methods, coordinate transformations, results derivations and averaging techniques.
Verification and Validation problems are presented to validate and
verify postprocessing displays using standard and widely accepted engineering problems. This is also a good source of example problems for learning to use the Results application.
CHAPTER 1
Introduction to Results Postprocessing
5
1.3
Result Definitions
In order to fully utilize the power of the postprocessor, a thorough understanding of how the results are stored and manipulated is important. To avoid confusion or the possibility of misinterpreting the graphical displays, the following definitions should be understood.
Result Types.
There are really only three results types, either scalar, vector, or tensor. Aside from these there are other aspects of results data as stored in the database that need to be understood. The following table summarizes these:
Term
Nodes/Elements
Scalar Results
Vector Results
Tensor Results
Real/Complex
Number
Load Case
Results Case
Result Type
Global Variables
Description
Results are associated with either nodes or with elements.
Single results values associated with either nodes or elements. They contain a magnitude only with no direction. Examples: strain energy, temperature, von Mises stress, etc.
Results values with three (3) components each associated with either nodes or elements. Vector results contain both magnitude and direction Examples: displacement, velocity, acceleration, reaction forces, etc.
Results values with six (6) components each (typically comprising the upper triangular portion of a symmetric matrix) associated with either nodes or elements. Examples: stress and strain components
Results stored as real numbers have only single values associated with any node or element. Complex numbers have two values associated with any node or element and are stored in the database as real and imaginary parts or magnitude and phase.
A group of applied loads and boundary conditions which may produce one or more result cases.
A collection of results as stored in the database (e.g., static analysis results, results from a load step in a nonlinear analysis, a mode shape from a normal mode analysis, a time step from a transient analysis, etc.).
Either scalar, vector, or tensor. Scalar results contain a magnitude with no direction such as temperature, strain energy, von Mises stress, etc. Vector results contain both magnitude and direction, such as displacement, velocity, and acceleration. Tensor results are symmetric with six unique values (xx, yy, zz, xy, yz, zx) such as stress or strain at a point. Each Results Case can have many Results types in them.
Values associated with results cases as a whole rather than to individual nodes and elements. Each result case may be associated with zero, one or more global variables, (e.g. time, frequency, load case, etc.).
1
1
6
PART 6
Results Postprocessing
Term
Primary Results
Layer Positions
Element Positions
Description
Physical quantities which may contain several different secondary result types. For example, stress is a primary result and von Mises stress is a derived or secondary result.
The location where element results are computed for plates and shells which may be homogenous or laminated. Other types of elements have a default non-layered ID. Beam results can also be layered. Examples are top, bottom, and middle results of plate elements, different locations in a beam cross section, etc.
The location within the element (at a particular layered position for plates, shells, and beams) where results are computed. These positions are the quadrature points, element centroid, or nodal points. For beam plots, results at intermediate points along the beam can also be displayed as long as the analysis code has computed results at those locations.
When postprocessing results, you should be able to answer these questions about any data that is to be evaluated:
•
Is the result type scalar, vector, or tensor?
•
Is the result associated with nodes or elements?
•
Is the result single-valued or complex (real/imaginary)?
•
What layer-position does the result belong to?
•
For element results, where in the element is the result computed?
Plot Definitions.
The Results application provides various different plot types for results visualization. These plots, sometimes referred to as tools or plot tools, allow graphical examination of analysis results using a variety of imaging techniques and also simultaneous display of multiple plots to aid in the understanding of interactions between results. The following table summarizes the plots available followed by a description of each.
Plot Type Description
Display of the model in a deformed state.
Fringe Plots
Contoured bands of color representing ranges of results value.
Colored contour lines representing result values.
Marker Plots
Colored scaled symbols representing scalar, vector and tensor plots.
Animation
Freebody Plots
Labels for scalar, vector or tensor quantities are displayed on the model at interactively selected entities.
Not technically a plot type, however most plot types can be animated in a modal or ramped style or in a transient state if more than one result case is associated with an particular plot type.
These are freebody diagrams plotted specifically from MSC.Nastran grid point force balance results.
CHAPTER 1
Introduction to Results Postprocessing
7
Plot Type
Graph (XY) Plots
Reports
Description
XY plots of results versus various quantities. Results can be plotted against other results values, distances, global variables or arbitrary paths defined by geometric definitions such as a curve.
Also not technically a plot type, however report definitions of results are stored in the database like any other plot tool type and can be created and modified to write reports to text files or to the screen.
Deformation
plots are used to display the current model and posted plot tools in a deformed state. Care must be taken when applying other plots on a deformation plot when more than one deformation plot is posted since multiple deformation plots can easily clutter the graphics. An optional display of an undeformed model is controlled as an attribute of the deformation tool.
The targeting of deformation tools to anything other than nodes and elements or groups of nodes and element is not allowable. Deformations may be used to display any nodal vector data.
Fringe
plots map color to surfaces or edges based on the result data defined for the tool. Fringes are developed from nodal-averaged scalar values. Fringes may be plotted on the model’s element faces or edges. The fringe tool will supersede all existing or default color and shading definition for the entities at which the fringe is targeted.
Contour Line
plots display contour lines representing result data selected. Contours line plots are developed from nodal-averaged scalar values. Contour lines may be plotted on the model’s element faces or edges.
Marker
plots display nodal or element based scalar, vector or tensor results as icons or arrows at the result locations. Markers may be targeted at model features such as nodes, corners, and edges or faces of elements. Individual scalar, vector and tensor plots are described below but are known generically as marker plots.
Cursor
plots display nodal or element based scalar, vector or tensor results as labels. There are three types of cursor plots: (1) Scalar, (2) Vector or (3) Tensor. Scalar, vector and tensor result quantities are displayed as one, three and six labels, respectively. Labels may be targeted at model features such as nodes and elements. Cursor plots are interactive and the labels are displayed on the model as the user selects the entities. The result value labels maybe displayed in a spreadsheet and written to a file, if desired.
Scalar
plots display nodal or element based scalar data and are considered special types of marker plots. Scalars may be colored and scaled based on value and may be targeted at various model features such as node, faces and edges of elements, and corners.
Vector
plots display nodal or element based vector data as component or resultant vectors and are considered special types of marker plots. Vectors may be colored and scaled based on magnitude and may be targeted at various model features such as node, faces and edges of elements, and corners.
Tensor
plots display an iconic representation of a symmetric tensor and are considered a special type of marker plot. Tensors may be oriented in the axes of principal stress or the tensor’s defined coordinate system. Tensors may be defined by element- or nodal-based tensor data.
Nodal tensors are mapped from element tensors and are used when a tensor marker tool is targeted at other tools. Tensors may be targeted at nodal- and element-based model features.
1
1
8
PART 6
Results Postprocessing
Animation
of most plot types is fully supported. Deformations can be animated in modal or ramped styles as well as true deformations from transient analyses. Animations from other plot types can accompany a deformation animation such as a stress field fringe plot or they can be animated separately from the deformation. Animation can be turned on or off from any existing plot or can be designated at creation time or when modifying a plot. The number of animation frames and other parameters such as the speed of animation are all easily controllable.
Freebody
plots display a freebody diagram on a selected portion of the model. The plots are in the form of vector plots showing either the individual components or resultant values.
Individual components that make up the total freebody diagram can also be plotted separately such as reaction forces, nodal equivalenced applied forces, internal element forces and other forces such as those from MPCs, rigid bars, or other external influences. New loads and boundary condition sets can be created from a freebody plot.
Graph
plots are XY plots generally consisting of a results value versus some variable such as time or frequency or possibly a model attribute such as distance from a hole or edge or another results value.
Plot Attributes.
The Results application provides the means of Creating, Modifying, Deleting,
Posting and Unposting these plots as well as means for dynamically manipulating these plots for interactive results imaging. Each plot created has assigned attributes which determine its characteristics. All plots have the following attributes.
Attribute
Name
Type
Result(s)
Target
Display
Attributes
Animation
Attributes
Posting Status
Description
A unique user-definable string descriptor to identify the plot tool. If no plot name is specified a default name is used. The default will be used each time unless the user specifically defines a unique name.
One of the plot tool types described in
A results case or a list of results cases and the corresponding result type which the plot tool is to display.
Onto where or to what entities the plot is to be displayed. This is either on a model feature such as nodes, elements, or on another plot tool.
Each plot type has specific settings to control how the plot is to be displayed. These include such things as component colors, titles, label, rendering styles and a myriad of other attributes.
Attributes to describe whether the tool is to be animated and how the results are to be mapped to animation frames. For instance, is the animation modal or transient and how many frames will be used for the animation?
Each plot is either Posted (displayed) or Unposted (not displayed) with the exception of reports.
Plot Targets.
Result plots may be displayed on selected model entities or other selected plot tools. The model based targets may be defined by a list of posted groups, by all posted entities in the current viewport, or by individual nodes or elements or by elements with certain attributes. The model entities and tools which may act as targets for Results application plots are described below.
CHAPTER 1
Introduction to Results Postprocessing
9
Elements
indicate that results will be displayed on all selected elements of the model. For graphs and reports the information can be extracted from the centroid, the element nodes or element data as stored in the database.
Free faces
describe those element faces common to only one element. This includes faces lining the outside surface of a model or those inside surfaces exposed to internal voids. Free faces are appropriate targets for displays such as fringe plots which are normally displayed on the surface of the model or on a cutting plane through the model.
All Faces
display results on each face of each element.
Free Edges
display results on edges common to only one element. Use this target type when displaying results on the same edges which are used to draw the model when Free Edge is selected as the finite element display method.
All Edges
display results on all element edges. Using this target selection allows mapping of results onto a wireframe representation of the model.
Nodes
display the selected results at each nodal location of the model. Tensor and vector plots may all be displayed at nodal locations.
Corners
display the selected results at nodes which are common to only one element. Tensor and vector plots may all be displayed at corner locations.
Paths
display the selected results along a defined path. The path can be defined as either a series of beams or element edges, geometric curves, or selected points (either geometric or FEM based).
This target type is used with Graphs plots.
The following table summarizes the valid targets for all plot tools. When specifying target entities in most cases you must specify both the target entities to which the plot will be assigned and the attributes or additional display information. The table below shows target entity versus attribute and which plots types are valid (D=deformation, F=fringe, Cl = Contour Lines, S=
Scalar, V=vector, T=tensor, Cu=Cursor, G=graph, R=report).
Attribute
1
Target
Current Viewport
D,S,V,T,R F,Cl,S
Nodes
Elements
Groups
Materials
,V,T
F F,S,V
,T
F F
F D,S, V,T,R S,V,
T
D,S,V,T,
Cu,G,R
F D,S,V,T,
Cu,G,R
D,S,V,T,G,
R
D,S,V,T,G,
R
F,Cl
F,Cl,S
,V,T
F,Cl,S
,V,T
F F,S,V
,T
F F,S,V
,T
F D,S,V,T,G,
R
S,V,
T
F D,S,V,T,G S,V,
T
R
R
G,R
G,R
1
10
PART 6
Results Postprocessing
Target
Attribute
Properties
Element Types
Paths
D,S,V,T,G,
R
F,Cl,S
,V,T
D,S,V,T,R F,Cl,S
,V,T
F F,S,V
,T
F F,S,V
,T
F D,S,V,T,G S,V,
T
F D,S,V,T S,V,
T
G
G,R
R
CHAPTER 1
Introduction to Results Postprocessing
11
Other Definitions
Post
Unpost
Range
Viewport Range
Auto Range
Extrapolation
Averaging
Derive
Term
Interpolation
Definition
To graphically display the plot or plots.
To remove the plot or plots from the graphical display.
A MSC.Patran database entity defined by a series of number and threshold values for each level within a range. Ranges are used to map spectrum colors to results values. A spreadsheet form is available to control range levels.
The range entity currently assigned to the MSC.Patran viewport.
A range which is not a database entity but is automatically calculated for a plot based on the results values. This type of range may be manipulated dynamically to change the range extremes and the number of intermediate levels.
Methods of converting results values from certain element locations to other locations (e.eg., converting results at Gauss points to nodal values).
Methods of converting several results associated to the same physical location to a single results value such as when results at nodes have contributions from all connected elements.
Methods of converting results values, for instance, when calculating von Mises stress from stress tensor components.
Methods of calculating new results values between existing locations of results values. For example: displaying more frames of animations than results cases available.
Methods of transforming results values with magnitude and direction attributes into alternate systems.
Coordinate
Transformation
More detailed information on the numerical methods can be found in
Results Label.
MSC.Patran displays results labels on plots so that all labels are started at the free end of the line segment (away from the node or element centroid); and continue to the right, independent of the arrow. Often the label is obscured.
For vector and tensor plots, you can now set the label to appear at the free end of the line segment, and position it so that it appears centered with respect to the arrow. All labels are pushed “away” from the segments (i.e., an arrow that goes from the screen center to the left will have the label end at the arrowhead instead of the begin at the arrowhead, as in the past). To enable the label placement feature, you need to add a preference to the Patran db using:
db_add_pref(524,2,0,TRUE,0.0,"")
db_set_pref_logical(524,TRUE) from the patran command window input text data box. This will remain in effect for the life of the database.
1
1
12
PART 6
Results Postprocessing
When the "VECTORTEXTCENTERED" preference (524) is in effect, the label text associated to results vectors, result tensors, lbc marker "arrows", property "arrows", and arrow created using
"gm_draw_result_arrow":
•
are not rendered until the end of the viewport rendering. The text that is attached to an arrow is drawn at a location so that the free end of the vector receives the text. The hang point of the text is translated (in the 2d world) such that the center of the box enclosing the text (text box) is contained in the line of the (2d) vector and the edge of the text box is just touching the free end.
•
are suppressed (not rendered) if the free end of the vector to which the text is attached is occluded. That is, if the z-depth of the device coordinate for the free endpoint is greater than the current z-depth for the device x,y (something eclipses the end of the vector tail) then the text is suppressed. This does not apply if the viewport was rendered entirely in wireframe mode. All vector text is considered visible if the viewport was rendered in wireframe mode.
CHAPTER 1
Introduction to Results Postprocessing
13
1.4
Capabilities and Limitations
The Results application provides the capabilities for Creating, Modifying, Deleting, Posting,
Unposting and manipulating results visualization plots as well as viewing the finite element model. In addition, results can be derived, combined, scaled, interpolated, extrapolated, transformed, and averaged in a variety of ways, all controllable by the user.
Control is provided for manipulating the color/range assignment and other attributes for plot tools, and for controlling and creating animations of static and transient results.
Results are selected from the database and assigned to plot tools using simple forms. Results transformations are provided to derive scalars from vectors and tensors as well as to derive vectors from tensors. This allows for a wide variety of visualization tools to be used with all of the available results.
Results imaging routines are optimized for graphical speed but may vary depending on hardware.
Please be aware of the following limitations or constraints:
•
When a Result Data quantity is deleted, it is deleted from all Results Cases that contain the Results Data quantity.
•
Transient animations are not possible from the Quick Plot form. They must be created under each specific plot type option (deformation, fringe, marker, etc.).
•
Multiple animations can be viewed simultaneously in a single viewport.
•
Only one spectrum and range can be associated to any one viewport at a time. If multiple plots are posted to a viewport, the spectrum and corresponding range will only be applicable to one of the posted plots. Values from other plots not corresponding to the posted range will take on the posted range’s spectrum. Values outside the range will appear as the highest or lowest range color. This may make some plots appear monochrome. This is done to avoid confusion and misinterpretation of result data.
•
It is not recommended to calculate invariants (e.g., von Mises) from complex results because the phase is not accounted for.
1
1
14
PART 6
Results Postprocessing
1.5
Using Results
The Results application is based on the creation and manipulation of results visualization plots.
The first action to be performed using Results is to create a plot, sometimes referred to as a tool or a plot tool. This however is transparent to the user when doing basic operations such as simple deformed plots, fringes, and animation. Each plot type has its own default settings and attributes which are set and modified when a user creates a plot. Only when these settings and attributes need to be saved and restored quickly for subsequent use does the user need to concern himself about physically saving the plots. This is done using the Create action on the main Results application form. Other actions are described in the following table, and summarized in this section.
Action Description
This action is used to create Results visualization plots sometimes referred to as tools. Creating a plot will result in a graphical display with the exception of creating reports and deriving results. If you try to create a plot that already exists, you will be prompted for overwrite permission.
Sometime it is necessary to select only certain Results Cases or to filter the Results Cases specifically for more precise control when creating plots. A special form allows you to do this easily and efficiently as well as view all Results Cases available to you.
This action is used to modify existing Results visualization plots or tools. This action performs identically to the Create action with the exception that no overwrite permissions will be asked if plot tools already exist that are being modified.
This action is used to graphically display (post) or graphically remove (unpost) existing Results display plots or ranges/spectrums from the computer screen. The plots and ranges are not physically removed from the database with this operation. Only their graphical display is recalled or removed.
This action is used to delete existing Results visualization plots and for deleting result cases and result data associated with result cases from the database. Use this option with care. Some operations may not be undoable.
There is a form which allows the currently posted spectrum to be changed and manipulated as well as deleted or new ones created.
There is also a form which allows for control over which range
(numbers) are assigned to newly created plots and also control over each color bar of the spectrum for the currently posted plot or plots.
See
These are forms for setting up and controlling certain aspects of an
CHAPTER 1
Introduction to Results Postprocessing
15
Create
Creating a plot generally involves four to six basic steps (although it may vary from plot type to plot type). For simple plots where it is acceptable to use all default values then the Quick Plot option is all that is needed. The icons on the top of the form give access to all controls necessary.
For full control of most plots the steps are:
Action:
Object:
Results Display
Create
Deformation
STEP 1:
Set the Action to Create and select an
Object (the plot type) from the Results application form.
STEP 2:
Select a Results Case from this listbox.
Select Result Case(s)
Load Case 1, Static Subcase
Select Deformation Result
Applied Loads, Translational
Displacements, Translational
Displacements, Rotational
STEP 3:
Select a result associated with the Results
Case from this listbox.
STEP 4:
Select the target entities to which the plot will be applied (optional).
STEP 5:
Set any plot attributes if necessary
(optional).
STEP 6:
Press the Apply button on the bottom of the form. The plot will be displayed.
1
Show As:
Animate
Resultant
-Apply-
Reset All
Plot Types:
•
•
•
•
•
Marker Plots (Scalar, Tensor, Vector)
•
•
•
•
•
Note:
A separate chapter is dedicated to describe in detail the creation and manipulation of each plot type.
Important:
Plots can be optionally named and saved in the database and subsequently recalled and graphically displayed. If no name is given, a default name is assigned. If a new plot is created without specifying a name, the default will be overwritten each time. Overwrite permission will be asked if a name is given and it already exists.
1
16
PART 6
Results Postprocessing
Selecting Results.
For all operations you must select results from a listbox. What results are displayed in this listbox is somewhat dependent on the result type (static, transient, etc.) or the number of subcases, time, frequency, or load steps associated with these results and how they have been filtered. When multiple subcases, time, frequency, or load steps are present, the display in the Select Result Cases listbox will display a title such as
LoadCase x, n of n subcases or something similar indicating that there are multiple sets of results for this Result Case.
When multiple results exist for any given Result Case, an additional button and toggle appear on the form. One allows for filtering and selecting the desired subcases which will appear selected in the listbox and the other determines the appearance of these multiple results in the listbox itself.
Action:
Object:
Results Display
Create
Fringe
This button icon brings up the Select Result Cases form to allow for selecting and filtering of the results cases based on various criteria such as a global variable (time). Once the filtering has been done only those results that passed the filter criteria will be selected for subsequent postprocessing.
See
Select Result Cases
Load Case 1, 1 of 41 Subcases
Select Deformation Result
Applied Loads, Translational
Displacements, Translational
Displacements, Rotational
This button icon changes the way the Result Cases are displayed in the listbox. If toggled OFF, every individual subcase, time, frequency, or load step will be visible in the listbox. If toggled ON, then only the title of the primary Result
Case will appear with a summary of how many subcases are associated with it based on the filter criteria. This is known as the abbreviated form.
This toggle will not appear unless Result Cases with multiple subcases exist. This is true also for the Select button icon.
Position...(At Z1)
Show As:
Resultant
Animate
-Apply-
Reset All
Additional results selection control is given when multiple layers exist.
Once Result Cases have been selected and filtered, the Result Case name will be updated to show how many subsets of that Result Case have been selected. The name will appear something similar to
LoadCase x, m of n subcases
. If the Abbreviate Subcases toggle is then turned OFF, only those subcases selected through the filtering mechanism will be highlighted in the listbox.
How to filter results is explained in
Be aware that when selecting multiple Result Cases, such as for a transient animation, that the selected result type to plot must exist in all Result Cases selected. Otherwise an error message will result and no plot will be displayed until the Result Case selection is modified to meet this criterion.
CHAPTER 1
Introduction to Results Postprocessing
17
Result Layer Positions.
When multiple layers exist in a given result type, this form may be invoked by pressing the Position button in the Results application when the mode is set to Select
Results. Layers may correspond to shell top/bottom, ply layups, or different element type results.
Select...
Positions
This form is accessible by pressing the Position button from the Select Results mode if multiple layers exist for a given result type.
At Point C
At Point D
At Point E
At Point F
At Z1
At Z2
Select the position(s) you wish to be used in any subsequent plot. You may select multiple layers for any single Result
Case or you may pick a single layer for use when a single or multiple Result Cases are selected.
1
Option: Maximum
Close
Set the option to search and extract result quantities when multiple layers or Result Cases have been selected. These options are explained in the table below.
Action
Maximum
Minimum
Average
Sum
Merge
Description
If multiple layers or multiple Result Cases have been selected, then this option will search through all layers/Result Cases and extract the maximum value encountered for the subsequent plot. The value used in the search is the Quantity selected for resolution such as von Mises for tensor results.
This is identical to Maximum except the minimum is extracted.
Instead of extracting a maximum or minimum, values are averaged from each layer or Result Case based on the Quantity selected and graphically reported. Averaging is only performed over the number of actual layers or Result Cases that contained results at any entity. That is if 4 layers were selected and node 1 had three layers of results and node 4 had four layers of results, node 1 would be averaged only over the three that actually existed and not the four selected.
This option simply sums all values of the requested Quantity from each layer or Result Case and reports that value in the subsequent plot.
This option will use the first existing value encountered from any particular layer or Result Case. For instance if both top and bottom stresses are selected then only the top will be reported. This is useful for layers that are associated with certain element types.
That way a layer with shells, a layer with solid, and a layer with beam elements can all be displayed simultaneously on the graphics screen in one operation.
1
18
PART 6
Results Postprocessing
Note that when performing maximum/minimum extractions or averaging and summing that the following procedures are performed in order:
1. The selected Quantity of interest is calculated for all layers or Result Cases selected, first performing any transformations, scaling, and averaging, or extrapolation as requested in the Plot Options. Quick Plot operations use standard defaults for all plot options.
2. Once the Quantity of interest is calculated for all selected layers or Result Cases, the maximum/minimum extraction, averaging or summation is performed and reported in the subsequent plot.
Note that this operation is different than what the results derivations do in
(p. 193). These operations are scalar based, meaning that the maximum,
minimum, average, or sum operations are done based on the requested scalar quantity.For instance, you would not be able to properly calculate von Mises stress at the neutral axis of a beam in pure bending by selecting the top and bottom layers and requesting an average where the expected von Mises stress should be zero. The von
Mises will be calculated at top and bottom and then averaged. For this type of operation where the components of a vector/tensor need to be averaged or summed before the requested result quantity is calculated or the vector/tensor components based on maximum or minimum comparisons of the requested scalar quantity are
Important:
It is important to note that if multiple Result Cases have been selected and only a single layer exists or has been selected that the default plot will result in a maximum plot of all selected results.
CHAPTER 1
Introduction to Results Postprocessing
19
Filtering Results.
Filtering results is accomplished from the Select Result Cases form which is accessible from the Results application when the first icon button
(Select Results) is active and multiple subcases exists. An icon button appears when Result Cases are in their abbreviated form to access the filter form which can also be accessed by clicking on the Result Case name.
Select Results Cases
Select Result Case(s)
Load Case 1, 41 subcases
Select a Result Case from this listbox which appears as a title with the number of subcases associated with the Result Case(s). Only one can be operated on at a time.
1
Filter Method:
Global Variable
Variable: Time
Values:
Above
Min: 0.
Value:
1
Max: 2.
Filter Clear
Selected Result Cases
Load Case 1, Time = 0.
Load Case 1, Time = 0.05
Load Case 1, Time = 0.1
Load Case 1, Time = 0.2
Load Case 1, Time = 0.3
Load Case 1, Time = 0.4
Load Case 1, Time = 0.95
Remove
Select a method of filtering. The methods to choose from are Global Variable, String, Subcase
Ids, and All. These are described in
Set the appropriate criteria depending on the
Filter Method above.
Filters the subcases. The listbox below will fill with the selected subcases.
Any subcases highlighted in the listbox below can be removed by using this button.
Clears the Selected Result Cases listbox.
Every time the Filter button is pressed, new results subcases will be added to whatever existing results are already selected. To do a new filter you must clear this listbox.
Apply Close
Makes the selected subcases active for postprocessing. The number of selected subcases will appear back on the main form. Use the Close button to close the form down.
This form is expandable to allow you to view the entire Result Case names and global variable if necessary.
1
20
PART 6
Results Postprocessing
The different filter methods are explained in
.
Method
Global Variable
String
Subcase IDs
All
Table 1-1 Filter Methods
Description
Any global variables associated with the selected Result Case will show up in the Variable option menu. Select the one you would like to filter with, change the criteria using the Value option menu and enter the value or range to filter by. Press the Filter button to complete the filter action. Press the Apply button at the bottom of the form to activate the filtered subcase selection.
Enter a string and use wild cards (the * character) to filter results.
For example if you wanted all subcases with the string Time in it then you would use *Time* as the string with wild cards on each end of the word. Press the Apply button at the bottom of the form to activate the filtered subcase selection.
Subcases can be filtered on Subcase IDs by entering the appropriate
IDs. To select separate IDs, separate them by spaces (1 3 5). To select a range use a colon between the numbers (1:5). To select by increments use two colons, for example: 1:10:2, which interpreted means select subcases one through 10 by twos. Or use any combination of spaces and colons between subcase IDs to select as many as you wish. Press the Apply button at the bottom of the form to activate the filtered subcase selection.
No filter method is selected. No options are available. Simply press filter and all subcases will be selected from whatever primary
Result Case is selected. Press the Apply button at the bottom of the form to activate the filtered subcase selection.
Important:
Only one Result Case can be filtered at a time. If you need to filter subcases from more than one Result Case then you will need to perform the operation once for each Result Case.
Note on Result Case Names:
By default if a Result Case has more than 30 subcases (time steps, load steps, etc.) then the
Result Case name will be displayed in an abbreviated form to reduce clutter in the listboxes. The default number at which this abbreviated form takes over can be changed with a settings.pcl
parameter: pref_env_set_integer( “result_loadcase_abbreviate”, 30 )
See
The settings.pcl file
(p. 41) in the MSC.Patran Reference Manual, Part 1: Basic Functions. It is possible to toggle back and forth from abbreviated form and full form at any time by pressing the icon button shown here.
CHAPTER 1
Introduction to Results Postprocessing
21
Default Settings.
For all modes of the Results application (selecting results, target entities, display attributes, plot options, and animation options) logical defaults have been set. In general, when an option on a form is changed, it remains until the user modifies or resets it. On the bottom of the Results application form is a Reset button that will restore default settings.
Pressing the Reset button only affects the particular plot type currently set.
1
-Apply-
Reset All
-Apply-
Reset
In the Select Results mode of the
Results application, the Reset All button will restore all default settings for any particular plot type. This includes target entities, display attributes, plot and animation options.
In any other mode of the Results application, the
Reset button will only restore that modes settings for any particular plot type.
In some instances it is possible to modify these defaults to the user’s preference. Not all default attributes and setting can be altered by the user since certain dependencies exist on result types and available options. However for display attributes, default setting may be altered in a template database. This template database can then be saved and made available to all users that wish to use the altered default attributes. See
The Template Database File (template.db)
(p. 47) in the MSC.Patran Reference Manual, Part 1: Basic Functions
In order to accomplish this, the standard MSC.Patran database is pre-loaded with invisible plot tools called
MSC_Initialize
. There is one for each plot type (Deformation, Fringe, Vector,
Tensor, Graph). This plot is never visible to the user but default display attributes are extracted from these plot tools.
Toggles the form to change display attributes for all plot types.
To modify the default display attributes, you simply need to modify the
MSC_Initialize
plot tool for the plot type in question. These basic steps need to be followed:
1. Open a MSC.Patran database that already has a model and results or simply create a
new database and model using Demo results (See
2. Create a plot of the type you wish to modify with the display attributes that you want.
A PCL command will be issued in the command line window of MSC.Patran. It will also be output to a session file typically called patran.ses.01
(the version number may vary).
3. Either edit the session file or edit the PCL command from the command line by replacing the plot name (which will probably be blank something like default_XXX where
XXX
is
Fringe
,
Tensor
,
Vector
, etc.) with the name
MSC_Initialize
. See the example below.
4. Also edit this PCL command such that it is a modify command as opposed to a create command.
5. Close down the current database and open a new blank database.
1
22
PART 6
Results Postprocessing
6. Run the edited session file or re-issue the PCL command to modify the
MSC_Initialize plot tool.
7. Save this database as the new template.db
.
Display attributes for this modified plot tool have now been set.
As an example, say that the default display attributes for a deformation plot are to be modified.
The following PCL command is issued when creating a deformation plot with the desired attributes: res_display_deformation_create(““,“Elements”,0,[““],9,[“DeformedStyle:White,Solid,1,Wire frame”,“DeformedScale:Model=0.1”,“UndeformedStyle:ON,Blue,Dash,1,Wireframe”,“TitleDispla y:ON”,“MinMaxDisplay:ON”,“ScaleFactor:1.”,“LabelStyle:Fixed,8,White,4”,“DeformDisplay:Re sultant”,“DeformComps:OFF,OFF,OFF”])
The PCL command should then be edited as follows: res_display_deformation_modify(“MSC_Initialize“,“MSC_Initialize”,“Elements”,0,[““],9,[“D eformedStyle:White,Solid,1,Wireframe”,“DeformedScale:Model=0.1”,“UndeformedStyle:ON,Blue
,Dash,1,Wireframe”,“TitleDisplay:ON”,“MinMaxDisplay:ON”,“ScaleFactor:1.”,“LabelStyle:Fix ed,8,White,4”,“DeformDisplay:Resultant”,“DeformComps:OFF,OFF,OFF”])
Note that the only modifications are to change the create to modify in the PCL function name and enter the name of the plot tool
MSC_Initialize
twice. This PCL command should then be issued either via a session file or directly from the command line after opening a new empty database.
The above example simply sets the undeformed line style to dashed as opposed to the standard solid line.
CHAPTER 1
Introduction to Results Postprocessing
23
Use Templates
This Action menu provides the means to select and use Results Templates to make Deformation
Plots, Fringe Plots, Marker Vector Plots, Marker Tensor Plots, Graphs, and Reports.
The menu is similar to the Create menus, except that the Results Display Attributes and Plot
Options icons and associated menus have been replaced with a Display Templates icon and associated menu. The Display Attributes and Plot Options values will be determined by the
Results Template selected instead of the many individual menu settings on the Display
Attributes and Plot Options forms of the Create menu.
For Results plots (Deformation, Fringe, Marker Vector and Marker Tensor) you may chose a title either from the template or as determined by the load selection on the Select Results form. Either can be edited once selected by the corresponding switch for “Title From:” “Template” or “Load
Selection”.
Graphs do not use titles.
Report Titles are accessed via the “Format…” button.
STEP 1:
Set the Action to Use Template.
1
STEP 2:
Select the type of plot for which you will use a template.
STEP 3:
Change the Result Cases and/or results type assigned to this plot (optional).
STEP 4:
Select to show as either Resultant or
Component.
STEP 5:
Press the Apply button on the bottom of the form.
1
24
PART 6
Results Postprocessing
Modify
Once a plot has been created, it may be modified using the Modify action on the Results application form. It is only necessary to actually modify a plot if it has been optionally named and saved in the database. Otherwise the Create action can be used exclusively. Default plots can be overwritten with the Create action. To modify a named plot, follow these general steps:
Action:
Object:
Results Display
Modify
Deformation
STEP 1:
Set the Action to Modify and select an Object
(the plot type) from the Results application form.
STEP 2:
Select the named plot to be modified.
STEP 3:
Change the Result Cases and/or results type assigned to this plot (optional).
Existing Deformation Plots...
STEP 4:
Change the target entities to which the plot will be applied (optional).
Select Result Case(s)
Load Case 1
Load Case 2
Load Case 3
STEP 5:
Modify the plot attributes and other options if desired (optional).
Select Deformation Result
Deformation, Translational
Deformation, Rotational
STEP 7:
Press the Apply button on the bottom of the form. The plot will be modified and displayed if not already.
Show As:
Animate
-Apply-
Resultant
Reset All
Note:
A separate chapter is dedicated to describe in detail the creation and modification of each plot type.
Plot Types:
•
•
•
•
•
Marker Plots (Scalar, Tensor, Vector)
•
•
•
•
•
Important:
It is suggested to only modify plots that have specifically been given names. It is not necessary to modify the default plots. Default names are given to the plots when no specific name is specified. The Create action continually overwrites these default plots with their corresponding names, therefore it is not necessary to use the Modify action on them.
CHAPTER 1
Introduction to Results Postprocessing
25
Post/Unpost
Posting and unposting of plots to the graphics viewport(s) can be performed. Posting or unposting of ranges and their corresponding spectrum is also allowable. See the next section
Posting/Unposting Plots.
Once a plot or set of plots has been created, they may be posted
(displayed) or unposted (removed) with the Post action on the Results application form. (This is also true for Ranges. See
(p. 29) for more detail. Multiple plots may be posted simultaneously. To post or unpost a plot,
do the following:
Action:
Object:
Results Display
Post
Plots
STEP 1:
Set the Action to Post and the Object to Plots from the
Results application form.
Existing Plot Types
DEF_default_Deformation
FRI_default_Fringe
VEC_default_Vector
STEP 2:
Select the plot(s) to be posted. Use the shift key to select multiple plots and/or the control key to select noncontinuous
selections.
1
These buttons either deselect all plots from the list box, select all plots in the listbox, or select only those plots posted to the current viewport. respectively.
Select None
Select All
Select Posted
-Apply-
STEP 3:
Press the Apply button on the bottom of the form.
The plots will be posted (displayed) and those that were deselected will be unposted.
When multiple viewports are in use, make sure that you make the viewport to which you want to post the plots active. The current viewport always has a red border around the graphics. To change the current viewport, place the cursor in the border of the graphics window (the cursor will change to hand icon) and click the mouse button. The Post/Unpost listbox plot will update itself to show what plots are posted to the currently active viewport.
By default all posted plots will be re-posted when a database is opened. This can be overridden by using a special setting parameter in the settings.pcl
file. The function is pref_env_set_logical(“result_dbopen_display”,TRUE/FALSE)
1
26
PART 6
Results Postprocessing
The default is TRUE. See
The settings.pcl file
(p. 41) in the MSC.Patran Reference Manual, Part 1:
Basic Functions.
Important:
Most plots can be targeted to or displayed on a deformed shape plot. When more than one deformation plot is posted, those plots that have been targeted at deformed plots will be displayed on all deformed plots that are posted unless specified differently under the Target Entities.
Posting/Unposting Ranges.
Each plot created is assigned a range according to the results values it is associated with. It is possible to put up multiple plots that are associated with varying types of results. It is possible that the result values from each plot vary by orders of magnitude
(displacement and stress for example). Posted plots will always take on the color spectrum currently posted. This means that some plots may turn monochrome if their results values are outside the range of the color spectrum posted. You may post and unpost the ranges associated with the various plots that are posted. Each posted plot associated to a color spectrum will be updated accordingly.
Results Display
Action:
Object:
Post
Ranges
STEP 1:
Set the Action to Post and the Object to Ranges from the Results application form.
Tool defining Viewport Range
FRI_stress
FRI_deformation
STEP 2:
Select the range to be posted. Only one range can be selected and posted at any one time. There will be a range for each plot posted unless deleted by the user.
This is a list of existing plot tools and not a list of actual ranges. The range associated with the selected plot tool will be assigned to the current viewport.
The plot whose range is currently displayed is noted at the bottom of the spectrum on the graphics window.
-Apply-
STEP 3:
Press the Apply button on the bottom of the form. The range will be posted (displayed) and posted plots will be updated to reflect the new range.
More information on how the Results application uses ranges can be found at the end of this
CHAPTER 1
Introduction to Results Postprocessing
27
Delete
Two items may be deleted: Plots and Results (see
Delete Plots.
Plots that have been created and stored in the database can be deleted and removed from the database.
Action:
Object:
Results Display
Delete
Plots
STEP 1:
Set the Action to Delete and the Object to Plots from the Results application form.
Existing Plot Types
DEF_default_Deformation
FRI_default_Fringe
VEC_default_Vector
STEP 2:
Select the plot(s) to be deleted. Use the shift key to select multiple plots and/or the control key to select noncontinuous selections.
1
-Apply-
STEP 3:
Press the Apply button on the bottom of the form.
The plots will be deleted.
1
28
PART 6
Results Postprocessing
Delete Results.
Results can be removed from the database with this function. Both Result
Cases and/or the results data associated with Result Cases can be deleted. Please note that any
Result Cases deleted will cause Result Case selections to be reset.
Action:
Object:
Results Display
Delete
Result Cases
STEP 1:
Set the Action to Delete and the Object to Result
Cases or Result Data from the Results application form.
Existing Result Cases
Load Case 1, Statics
Load Case 2, Statics
Load Case 3, Statics
STEP 2:
Select the Result Cases to be deleted. Use the shift key to select multiple plots and/or the control key to select noncontinuous selections. If results data is being deleted, select all the results data and the Result Cases from which the results data are to be deleted.
-Apply-
STEP 3:
Press the Apply button on the bottom of the form.
The results will be deleted.
CHAPTER 1
Introduction to Results Postprocessing
29
Spectrum/Range Control
A range is a set of numbers or range of numbers each assigned a specific color to be displayed in the viewport on a color spectrum bar. The colors in the spectrum bar and the number of ranges assigned to them correspond to the color bands plotted graphically on the finite element model to indicate levels of stress, displacement or other results quantities.
Selecting and manipulating the active range and/or spectrum is done in the Ranges and
Spectrums forms, which are accessible by two different methods. Most plot types allow for manipulation of the range and spectrum directly from their Display Attributes form:
Action:
Object:
Results Display
Create
Fringe The Display Attribute icon for most plot types will allow access to manipulate the spectrum and range assigned to the current viewport.
1
Show Spectrum
Spectrums...
Ranges...
The Spectrum button will bring up the
Spectrums form which allows for creation or assignment of a new spectrum to the current viewport. See
Display>Spectrums
(p. 330) in the MSC.Patran Reference
Manual, Part 1: Basic Functions
.
The Ranges button will bring up the Set Range form which will allow for assignment of a new range to the current viewport and spectrum.
Set Range
Select Fringe Range fringe_range standard_range
These two toggles, if ON, will allow the range values to be overwritten each time a new results quantity is plotted and post that range to the viewport, respectively. If you have created a special range and you do not wish its values to be overwritten, then turn the first toggle OFF.
Overwrite Range Values
Post Range to Viewport
Define Range...
The Define Range button will bring up the
Ranges form for definition of new ranges.
Display>Ranges
(p. 331) in the
MSC.Patran Reference Manual, Part 1: Basic
Functions
.
OK
Access to the Spectrum and Range forms is also available under the Display pull-down menu on the main MSC.Patran form. Creation and modification of the actual spectrums and ranges is done in these forms which are described in
Display>Ranges
(p. 331) and
Display>Spectrums
(p. 330) in the MSC.Patran Reference Manual, Part 1: Basic Functions.
1
30
PART 6
Results Postprocessing
Things to note about ranges for the various types of result plots:
1. By default, a new range will be assigned to every plot created if an existing one has not been selected. The range will be assigned to the current viewport. The name of the range will be the plot type with the plot name concatenated, e.g., FRI_ default_Fringe
,
VEC_ myvector
.
2. If you wish to assign a certain range to a new plot at creation time, simply select the range from the listbox as shown on the previous page. The range will remain as defined unless the Overwrite Range Values toggle has been set ON. If ON, then new maximum and minimum values will be calculated based on the result values and a new range calculated for the selected named ranged. This will permanently change the range until changed again; so care should be taken when using this option. This is true under the
Modify Action also.
3. Although many plots may be displayed simultaneously, only one spectrum and range is available for display in the current viewport at any one time. By default the range of the last plot created or posted will be displayed. Any existing, posted plots will take on the color spectrum of the posted range. This can cause some plots to appear monochrome indicating that their result values are outside the range of the current spectrum, either above or below it. This is done to avoid confusion and misinterpretation of results.
4. Any existing range may be selected as being the active range by posting it to the screen.
There are two ways to change the current range posted to any particular viewport. The first is under Viewport/Modify on the main MSC.Patran form. See
Viewport>Modify
(p. 268) in the MSC.Patran Reference Manual, Part 1: Basic Functions. Using the
Viewport/Modify or Range Update forms will assign the range to the currently posted plots (The spectrum legend can also be controlled. The second method is done directly
in the Results application under the Post/Ranges action/object. See
(p. 25). A list of ranges is not supplied here, but a list of posted plots. By selecting one
of the posted plots, its assigned ranged will be posted. Any other plots posted will update to reflect the posted range.
5. If you delete a plot, the associated range with the same name will NOT also be deleted.
You will need to physically delete it under the Define Range form.
CHAPTER 1
Introduction to Results Postprocessing
31
1.6
Results Title Editor
Results attributes forms that contain the Title Editor… or Results Title Editor button shown below open the Results Title Editor form when the button is pressed. If the Lock Titles checkbox is checked, the Title Editor button label changes to indicate that the Results Title Editor form will be opened in a readonly mode. In readonly mode the title may be viewed but not edited and the only active button is Cancel.
1
The readonly version of the Results Title Editor form is shown below.
1
32
PART 6
Results Postprocessing
The writable version of the Results Title Editor form is shown below.
Sample Title
Action
Title Selection
The Results Title Editor form has three main regions. Each region, and its usage are described below.
The Sample Title textbox shows the current title similar to how it will look on the Results plot.
If the Main Title variable is enabled, the string <Main Title> is shown to indicate that the main title will appear. The Main Title is the first title line. It includes the MSC.Patran version and the date and time of the plot.
Any enabled Results variables, are replaced by the Variable description shown in the Title
Selection region. Any enabled pre-text or post-text is shown as it appears in the Title Selection region. Any variables with enabled As Is/NA have (AsIs/NA) appended to the variable description. Any enabled new lines cause a new line to be started.
The text in this region is updated each time a change is made in the Title Selection region, either by switching a toggle or by pressing the keyboard Enter button while focus is in one of the databoxes.
CHAPTER 1
Introduction to Results Postprocessing
33
This textbox is readonly, however the cursor may be used to set the insertion position, which is then used as the insertion point for subsequently enabled variables. This procedure is explained in the Variable Insert Location section.
1
The Title Selection region is where most of the user interaction will occur. Control over which variables and text are included in the title is provided here. At the top of this region a set of column headings describe the meaning of the items in the rows below. Due to the number of items, a scrollframe is used to keep the form size reasonable. The scrollframe has three regions each with a line separator. At the top there are controls to set all of the toggles in the middle region either ON or OFF. Controls for all variables except Main Title are in the middle region.
The bottom region provides control for the Main Title and two General Text entries.
The toggles in the Show column control the display of the information in each row. If the toggle is off in a row, none of the information in that row is shown. If a toggle is on, the enabled information in that row is shown. The toggles in the Show Pre-text column control the display of any text entered in the corresponding Pre-text databox. The databoxes in the Pre-text column provide a means of entering text to precede each variable. In a given row, if the Show toggle and the Show Pre-text toggle are enabled, the text in the Pre-text databox will be inserted before the variable. The text in the Variable column provides an easy-to-recognize meaning for the variable in each row. It is also the text that appears in the Sample Title as the variable value.
The toggles in the Show Post-text column control the display of any text entered in the corresponding Post-text databox. The databoxes in the Post-text column provide a means of entering text to follow each variable. In a given row, if the Show toggle and the Show Post-text toggle are enabled, the text in the Post-text databox will be inserted after the variable.
Show As Is/NA only comes into consideration if a variable’s value is AsIs or blank “”. The toggles in the Show As Is/NA column control the display of the value of certain variables depending on their value. For example, if the Averaging Domain value is blank "" or AsIs, its value will not be shown unless its Show As Is/NA toggle is enabled. Note that many of the variables do not have a Show As Is/NA toggle. This is because a value of AsIs has no meaning for these variables.
The toggles in the New Line column control the insertion of new line control variables. In a given row, if the Show toggle and the New Line toggle are enabled, a new line will be inserted after the variable and its post-text. Note that there is a 10-line limit to Results titles, which limits the number of new lines to nine. A counter is provided next to the New Line column heading for reference. No more than nine new lines will ever be entered into the title. No more than nine
New Line toggles will ever be enabled in rows that also have the Show toggle enabled. Enabled
New Line toggles in rows with disabled Show toggles do not affect the count.
1
34
PART 6
Results Postprocessing
All of the Show, Show Pre-text, Show Post-text and Show As Is/NA toggles in the middle region of the scrollframe may be turned ON or OFF by using the toggles labeled All in the top scrollframe region.
The bottom scrollframe region provides control for the Main Title and two General Text entries.
The Main Title has already been described. The General Text entries provide a means of adding text to the title that is not associated to any variable. The General Text Start entry will appear at the start of the title while the General Text End entry will appear at the end of the title. Their
Show toggles control their display.
When its parent form opens the Results Title Editor form, the current title is decoded and the
Title Selection region toggles and databoxes are set. If no variables are found, the entire title is entered into the General Text Start databox.
The Action region has five buttons. The Defaults button sets the title to the default variables, pre-text’s, post-text’s, AsIs/NA and new line settings for the Results tool type. All current settings are overwritten. The Apply button applies the current title selection to the Results tool and leaves the form open. The OK button applies the current title selection to the Results tool and closes the form. The Apply button on the Attributes form must be selected to see the title update in the graphics viewport. The Reset button resets the title to the variables, pre-text’s, post-text’s, AsIs and new line settings it had when the form was last opened or when the Apply button was last selected. The Cancel button closes the form with no effect.
The settings.pcl preference: pref_env_set_string( "results_title_editor_defaults", "my_defaults" ) may be used to override the standard defaults. If defined, and the function specified exists, the function will be called whenever the Defaults button is pressed. The prototype for this function is given below. An example of this function will be provided.
Variable Insert Location
Variables are inserted based on the current insert location. The insert location can be changed by placing the cursor into the Sample Title textbox and clicking to set the insertion point. The insertion point is indicated by a vertical bar. The editor determines which variable the insertion point is in. The insertion of a new variable will be immediately after the variable containing the
CHAPTER 1
Introduction to Results Postprocessing
35
insertion point. If the insertion point is never set, it will be at the end. If the insertion point is placed at the beginning of the textbox, the next variable inserted will be at the beginning.
Turning a variable off and then on will remove it and then insert it back into its previous location. The insertion point is automatically updated such that subsequent insertions are placed after the previously inserted variable.
User-defined Defaults Function
To provide maximum flexibility to the user, a user-defined function may be provided to override any and all of the default title settings. Placing the following definition in the MSC.Patran settings.pcl file specifies a user-defined function.
pref_env_set_string( "results_title_editor_defaults", "my_defaults" )
Where my_defaults
is the name of a function. If the results_title_editor_defaults
preference is defined, and the specified function exists, the function will be called whenever the Defaults button is pressed. The prototype for this function is shown below. An example of this function will be provided.
FUNCTION my_defaults( tool_class, var, description, show, showPrefix, prefix, @
showSuffix, suffix, asIs, position, newLine )
/*
* FUNCTION my_defaults
* Returns default values for a given input variable.
* All output variable values will already have been set to the Patran defaults.
* This function needs only to modify those that the user wants modified.
*
* Input
* tool_class_in class name of tool type (default == Fringe)
* One of the following from "res_1_5_include.h":
*
* #define RES_TOOL_DEFORM_ATTR_CLASS_Q "res_display_def_attr"
* #define RES_TOOL_FRINGE_ATTR_CLASS_Q "res_display_fri_attr"
* #define RES_TOOL_2DCONTOUR_ATTR_CLASS_Q "res_display_cont_attr"
* #define RES_TOOL_3DCONTOUR_ATTR_CLASS_Q "res_display_cont_3d_attr"
* #define RES_TOOL_VECTOR_ATTR_CLASS_Q "res_display_vec_attr"
* #define RES_TOOL_TENSOR_ATTR_CLASS_Q "res_display_ten_attr"
* #define RES_TOOL_CURSOR_ATTR_CLASS_Q "res_display_cur_attr"
*
* var A variable name
* One of the following from "res_display.h":
*
* #define RES_DISP_TITL_VAR_DATE2 "$DATE2"
* #define RES_DISP_TITL_VAR_DATE "$DATE"
* #define RES_DISP_TITL_VAR_TIME "$TIME"
* #define RES_DISP_TITL_VAR_PRODUCT "$PRODUCT"
* #define RES_DISP_TITL_VAR_PROD "$PROD"
* #define RES_DISP_TITL_VAR_DB_NAME "$DB_NAME"
* #define RES_DISP_TITL_VAR_DB_PATH "$DB_PATH"
* #define RES_DISP_TITL_VAR_JOB_NAME "$JOB_NAME"
* #define RES_DISP_TITL_VAR_CODE_NAME "$CODE_NAME"
* #define RES_DISP_TITL_VAR_GV "$GV"
* #define RES_DISP_TITL_VAR_LC_NAME "$LC_NAME"
* #define RES_DISP_TITL_VAR_SC_NAME "$SC_NAME"
* #define RES_DISP_TITL_VAR_PRES_NAME "$PRES_NAME"
* #define RES_DISP_TITL_VAR_SRES_NAME "$SRES_NAME"
* #define RES_DISP_TITL_VAR_LYR_NAME "$LYR_NAME"
* #define RES_DISP_TITL_VAR_LOCATION "$LOCATION"
* #define RES_DISP_TITL_VAR_PLOT_TYPE "$PLOT_TYPE"
* #define RES_DISP_TITL_VAR_DATA_TYPE "$DATA_TYPE"
* #define RES_DISP_TITL_VAR_DERIVATION_L "$DERIVATION_L"
* #define RES_DISP_TITL_VAR_DERIVATION "$DERIVATION"
* #define RES_DISP_TITL_VAR_COORD_TRANS "$COORD_TRANS"
1
1
36
PART 6
Results Postprocessing
* #define RES_DISP_TITL_VAR_EXTRAP_METH "$EXTRAP_METH"
* #define RES_DISP_TITL_VAR_AVG_DOM "$AVG_DOM"
* #define RES_DISP_TITL_VAR_AVG_METH "$AVG_METH"
* #define RES_DISP_TITL_VAR_SCALE_FACT "$SCALE_FACT"
* #define RES_DISP_TITL_VAR_FILTER "$FILTER"
* #define RES_DISP_TITL_VAR_CUR_GROUP "$CUR_GROUP"
* #define RES_DISP_TITL_VAR_FRINGE_STYLE "$FRINGE_STYLE"
*
* Output
* description description (text that appears under "Variable" label)
* show controls whether variable is shown
* showPrefix controls whether prefix is shown
* prefix prefix
* showSuffix controls whether suffix is shown
* suffix suffix string
* asIs controls whether asIs is shown
* position position of variable in title starting with 1
* newLine controls whether a new line will follow the variable
*/
STRING tool_class_in[], var[], description[], prefix[], suffix[]
LOGICAL show, showPrefix, showSuffix, asIs, newLine
INTEGER position
Examples of User-defined Defaults Function
Two examples of user-defined functions are given in this section. The first is simple and changes only a few defaults. The second is more complex, and is similar to the function used by
MSC.Patran. See the section
User-defined Defaults Function
(p. 35) for a description of the
function arguments.
To use the simple function, place the following definition in the MSC.Patran settings.pcl file: pref_env_set_string( "results_title_editor_defaults", @
" simple_user_default_function " ) and make the function available by either compiling it in MSC.Patran using !!input or compiling it outside of MSC.Patran into a .plb and using !!library in MSC.Patran.
FUNCTION simple_user_default_function( @ tool_class_in, var, description, show, @
showPrefix, prefix, showSuffix, suffix, @
asIs, position, newLine )
STRING tool_class_in[], var[], description[], prefix[], suffix[]
LOGICAL show, showPrefix, showSuffix, asIs, newLine
INTEGER position
/*
* Simply change the prefix and description of
* some of the variables.
*/
SWITCH( var )
CASE( RES_DISP_TITL_VAR_CODE_NAME )
prefix = "My Language A Code:"
description = " My Language Code Name"
CASE( RES_DISP_TITL_VAR_CUR_GROUP )
prefix = " My Language Group:"
description = " My Language Group"
CASE( RES_DISP_TITL_VAR_DB_NAME )
prefix = " My Language DbName:"
description = " My Language Database Name"
CASE( RES_DISP_TITL_VAR_DB_PATH )
prefix = " My Language DbPath:"
description = " My Language Path Name"
END SWITCH
CHAPTER 1
Introduction to Results Postprocessing
37
1
END FUNCTION
To use the complex function, place the following definition in the MSC.Patran settings.pcl file: pref_env_set_string( "results_title_editor_defaults", @
" complex_user_default_function " ) and make the function available by either compiling it in MSC.Patran using !!input or compiling it outside of MSC.Patran into a .plb and using !!library in MSC.Patran.
FUNCTION complex_user_default_function( tool_class_in, var, description, show, @
showPrefix, prefix, showSuffix, suffix, @
asIs, position, newLine )
STRING tool_class_in[], var[], description[], prefix[], suffix[]
LOGICAL show, showPrefix, showSuffix, asIs, newLine
INTEGER position
STRING tool_class[MAX_TEXT_LENGTH]
SWITCH( tool_class_in )
CASE( RES_TOOL_FRINGE_ATTR_CLASS_Q, @
RES_TOOL_DEFORM_ATTR_CLASS_Q, @
RES_TOOL_2DCONTOUR_ATTR_CLASS_Q, @
RES_TOOL_3DCONTOUR_ATTR_CLASS_Q, @
RES_TOOL_VECTOR_ATTR_CLASS_Q, @
RES_TOOL_TENSOR_ATTR_CLASS_Q, @
RES_TOOL_CURSOR_ATTR_CLASS_Q, @
RES_TOOL_CURSOR_ATTR_CLASS_Q )
tool_class = tool_class_in
DEFAULT
tool_class = RES_TOOL_FRINGE_ATTR_CLASS_Q
END SWITCH
/* These are the most common. */
show = TRUE
showPrefix = FALSE
showSuffix = TRUE
suffix = ", "
asIs = FALSE
position = 0
newLine = FALSE
/* Set show. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_CODE_NAME, @
RES_DISP_TITL_VAR_CUR_GROUP, @
RES_DISP_TITL_VAR_DB_NAME, @
RES_DISP_TITL_VAR_DB_PATH, @
RES_DISP_TITL_VAR_DATE, @
RES_DISP_TITL_VAR_DATE2, @
RES_DISP_TITL_VAR_FRINGE_STYLE, @
RES_DISP_TITL_VAR_GV, @
RES_DISP_TITL_VAR_JOB_NAME, @
RES_DISP_TITL_VAR_PRODUCT, @
RES_DISP_TITL_VAR_PROD, @
RES_DISP_TITL_VAR_DATA_TITLE, @
RES_DISP_TITL_VAR_SCALE_FACT, @
RES_DISP_TITL_VAR_TIME )
show = FALSE
1
38
PART 6
Results Postprocessing
CASE( RES_DISP_TITL_VAR_FILTER )
IF( tool_class == RES_TOOL_DEFORM_ATTR_CLASS_Q ) THEN
show = FALSE
END IF
END SWITCH
/* Set showPrefix. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_AVG_DOM, @
RES_DISP_TITL_VAR_AVG_METH, @
RES_DISP_TITL_VAR_COORD_TRANS, @
RES_DISP_TITL_VAR_CUR_GROUP, @
RES_DISP_TITL_VAR_DATA_TYPE, @
RES_DISP_TITL_VAR_EXTRAP_METH, @
RES_DISP_TITL_VAR_FILTER, @
RES_DISP_TITL_VAR_FRINGE_STYLE, @
RES_DISP_TITL_VAR_GV, @
RES_DISP_TITL_VAR_JOB_NAME, @
RES_DISP_TITL_VAR_LOCATION, @
RES_DISP_TITL_VAR_SCALE_FACT )
showPrefix = TRUE
END SWITCH
/* Set asIs. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_AVG_DOM, @
RES_DISP_TITL_VAR_AVG_METH, @
RES_DISP_TITL_VAR_COORD_TRANS, @
RES_DISP_TITL_VAR_EXTRAP_METH, @
RES_DISP_TITL_VAR_FILTER )
asIs = TRUE
END SWITCH
/* Set position. */
SWITCH( tool_class )
CASE( RES_TOOL_DEFORM_ATTR_CLASS_Q )
SWITCH( var )
CASE( RES_DISP_TITL_VAR_PLOT_TYPE )
position = 1
CASE( RES_DISP_TITL_VAR_LC_NAME )
position = 2
CASE( RES_DISP_TITL_VAR_SC_NAME )
position = 3
CASE( RES_DISP_TITL_VAR_PRES_NAME )
position = 4
CASE( RES_DISP_TITL_VAR_SRES_NAME )
position = 5
CASE( RES_DISP_TITL_VAR_LYR_NAME )
position = 6
CASE( RES_DISP_TITL_VAR_LOCATION )
position = 7
CASE( RES_DISP_TITL_VAR_DATA_TYPE )
position = 8
CASE( RES_DISP_TITL_VAR_COORD_TRANS )
position = 9
CASE( RES_DISP_TITL_VAR_EXTRAP_METH )
position = 10
CASE( RES_DISP_TITL_VAR_AVG_DOM )
position = 11
CASE( RES_DISP_TITL_VAR_AVG_METH )
position = 12
CHAPTER 1
Introduction to Results Postprocessing
39
END SWITCH
DEFAULT
SWITCH( var )
CASE( RES_DISP_TITL_VAR_PLOT_TYPE )
position = 1
CASE( RES_DISP_TITL_VAR_LC_NAME )
position = 2
CASE( RES_DISP_TITL_VAR_SC_NAME )
position = 3
CASE( RES_DISP_TITL_VAR_PRES_NAME )
position = 4
CASE( RES_DISP_TITL_VAR_SRES_NAME )
position = 5
CASE( RES_DISP_TITL_VAR_DERIVATION_L )
position = 6
CASE( RES_DISP_TITL_VAR_LYR_NAME )
position = 7
CASE( RES_DISP_TITL_VAR_LOCATION )
position = 8
CASE( RES_DISP_TITL_VAR_DATA_TYPE )
position = 9
CASE( RES_DISP_TITL_VAR_COORD_TRANS )
position = 10
CASE( RES_DISP_TITL_VAR_EXTRAP_METH )
position = 11
CASE( RES_DISP_TITL_VAR_AVG_DOM )
position = 12
CASE( RES_DISP_TITL_VAR_AVG_METH )
position = 13
CASE( RES_DISP_TITL_VAR_FILTER )
position = 14
END SWITCH
END SWITCH
/* Set show suffix. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_LYR_NAME, @
RES_DISP_TITL_VAR_FILTER )
showSuffix = FALSE
CASE( RES_DISP_TITL_VAR_AVG_METH )
IF( tool_class == RES_TOOL_DEFORM_ATTR_CLASS_Q ) THEN
showSuffix = FALSE
END IF
END SWITCH
/* Set suffix. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_PLOT_TYPE )
suffix = ": "
CASE( RES_DISP_TITL_VAR_GV )
suffix = "Mode ,"
END SWITCH
/* Set newLine. */
SWITCH( var )
CASE( RES_DISP_TITL_VAR_LYR_NAME )
newLine = TRUE
END SWITCH
END FUNCTION
1
1
40
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
2
Quick Plots
■
■
■
■
2
32
PART 6
Results Postprocessing
2.1
Overview
Quick Plot is the default object of the Create action in the Results application and is designed to meet the needs of 80-90% of all postprocessing.
Quick Plot allows a user to quickly display a deformed plot, a scalar fringe plot, or a modal or ramped style animation. Both vector and scalar data can be animated, either separately or simultaneously. Transient animations are not supported from Quick Plot. For transient animations or more complicated postprocessing needs such as coordinate transformations or other derivations, the user will need to change the object to the specific type of plot to be created.
Quick Plot is designed to use all default settings for display attributes, target entities, and other options. By default the plot will display on everything posted in the current viewport. The display attributes for deformations, fringe plots and animations are also the default settings
used under the Display Attributes forms for deformations
plots.
Animation defaults are explained later in this chapter. See
The goal of Quick Plot is to give the user a quick, meaningful plot without having to worry about making sure all attributes, settings, and coordinate transformations are set properly. When fringe plots of element components are displayed using Quick Plot, the component data is oriented in a reasonable coordinate system to assure a meaningful plot whenever possible. The definitions of reasonable coordinate systems are as follows:
1. Element based result component data will be left in the coordinate system in which they were imported with the exception of two dimensional elements (plates, shells) that are oriented in an element connectivity based system. In this particular case, the component data will be transformed to the Projected Global system for fringe plot display.
2. For one dimensional (1D) and three dimensional (3D) elements, the Projected Global system is the Global system and therefore no projection is performed.
3. If data are in an Unknown coordinate system, no transformation will occur. If the
Unknown system happens to be an element system, then nodal averaging may not be correct, resulting in a meaningless plot. This puts the burden on the user to ensure correctness.
4. If data are in the Global system, a user defined Local, or an analysis specific projected system, then no transformations will occur.
5. Nodal based results are not effected by any transformations.
For more detailed definition of these coordinate systems see
Display attributes are accessible from Quick Plot for modification as explained in the next section.
CHAPTER 2
Quick Plots
33
No modifications can be made directly in Quick Plot for other plot options such as coordinate transformations as explained above. However you can change the Quick Plot default for two commonly used parameters. These parameters are the Coordinate Transformation and the
Averaging Method. They are modified in the settings.pcl
file. See
The settings.pcl file
(p. 41) in the MSC.Patran Reference Manual, Part 1: Basic Functions.
For Coordinate Transformations use the setting pref_env_set_string( “result_quick_transform”, “Default”)
Valid values are
Default
,
Global
,
CID
,
ProjectedCID
,
None
,
Material
,
ElementIJK
.
To change the default Averaging Method, use the setting pref_env_set_string( “result_quick_avg_method”, “DeriveAverage”)
Valid values are
DeriveAverage
,
AveragDerive
,
Difference
,
Sum
.
2
2
34
PART 6
Results Postprocessing
2.2
Quick Plot Usage
This is the default form that appears when the Results application is selected. Use this form to plot fringes, deformations and do simple animations.
The default appearance of this form is as shown to allow selection of results for subsequent plotting. The form can also be changed by selecting the right most icon from which animation options can be set. Selecting the left most icon will toggle the form back to select results. See
Results Display
Action:
Create
Object:
Quick Plot
These two button icons are for access to Display Attribute
and
Select the desired Result Case. This will fill out the Fringe
Result and Deformation Result listboxes below. If this listbox is empty, no results exist in the database. Results are imported from the Analysis application.
Select Result Cases
Default, Static Subcase
Select Fringe Result
Applied Loads, Translational
Bar Forces, Rotational
Bar Forces, Translational
Bar Forces, Warping Torque
Position...(at Z1)
Quantity: von Mises
Select a result type from which to make a fringe plot, if desired.
If layered results exist a subordinate form of the existing layer positions can be opened. See
A menu to display the valid transformation derivations. Used when a Vector or Tensor result is chosen in the Fringe Result listbox above. If the selected fringe result is a scalar value, this menu does not appear.
The possible transformations are
:
1. Vector to Scalar: Magnitude, X component, Y comp., Z comp.
2. Tensor to Scalar: von Mises, XX, YY, ZZ, XY, YZ, XZ, Minor,
Intermediate, Major, Hydrostatic, 1st Invariant, 2nd
Invariant, 3rd, Invariant, Tresca, Max Shear, Octahedral.
Be aware that for certain element based results, coordinate transformations may automatically occur to produce a
Select Deformation Result
Applied Loads, Translational
Constraint Forces, Translation
Displacements, Translational
Animate
-ApplyReset All
Select a displacement results from which to make a deformation plot, if desired. If a fringe plot is also selected, it will appear on the deformed structure.
When toggled ON, the selected results will be animated.
When the Animate toggle is turned ON, this button appears for selecting animation options. These are described in
(p. 37). It is not necessary to open this
subordinate form to create an animation. Defaults will be used.
Creates the plot and/or animation. The Apply button can be pressed with the form in either state (results selection or animation options).
More details follow on the next page.
CHAPTER 2
Quick Plots
35
For more information on the use of these button icons, see the appropriate section.
Fringe
Deformation
The derivation of each scalar quantity from either a tensor or vector that is available in the Quick
Plot application is described in detail in
It is important to note also that when deriving a scalar quantity for a fringe plot from an element based vector or tensor that results are averaged at the nodes due to the contributions from the surrounding elements. The default is to derive the desired quantity from the tensor or vector quantities (such as von Mises), then to average at the nodes. By default the averaging is done over all entities. This default Averaging Method can be changed with a settings.pcl
parameter.
When multiple layers exist for a specific Result Case and quantity, five additional options are also presented to the user from the Position button. These are Maximum, Minimum, Average,
Sum, and Merge. By selecting one of these layers, the minimum, maximum, average, sum or merging of all layers will be calculated for display in the subsequent plot. These plots may be more computationally intensive and take longer to display the final plot due to the results extraction of the maximum, minimum or average for all layers. The results of these derivations are not stored in the database. Use the Create/Results action and object to perform this task. See
Fringe plots and deformation plots created from the Quick Plot form are assigned default names that can be seen when the object is changed to Deformation or Fringe or from the Post and Delete forms. These names are default_Deformation
and default_Fringe
. The Quick Plot form will always operate on these named plots. If more than one viewport is open then the default names are incremented such as default_Deformation
2, default_Deformation
3, etc.
2
2
36
PART 6
Results Postprocessing
2.3
Animation Notes
There are two forms for controlling animations from the Results Quick Plot form and the manner in which the animations display on the graphics screen. These forms are described in this section. Transient animations are not allowed from the Quick Plot form.
The first form is for controlling animation attributes, such as the number of frames, or the animation method and is invoked before an animation is created. This form is described in
The second form is for actual control of the animation as it is animating and is the same for all animations. It is described fully in
(p. 158). The form remains on the screen
until either the Cancel button is pressed or the user presses the Abort (the hand) or Cleanup (the broom) icons on the main form.
CHAPTER 2
Quick Plots
37
Animation Options
This form is accessible from the Quick Plot form in the Results application when the Animate toggle is turned ON. It allows for modification of the display attributes of the animation before the animation is created. The default setting is shown in the following form.
If this toggle is OFF and a fringe result has been selected to animate with a deformed shape, the resulting fringe plot will appear static during the animation. It will not change from frame to frame. If ON, it will change frame to frame if a fringe result has been selected from the Quick
Plot form. The default is ON.
2
Action:
Object:
Results
Create
Quick Plot
Animate Fringe
Animate Deformation
Animation Method
Modal Ramped
Animation Graphics
2D
3D
Preview
MPEG
VRML (Max 120 Frames)
Default Window Size
Number of Frames
Apply
8
If this toggle is ON, then the deformation results selected will animate (change from frame to frame). If OFF, it will not animate. This is really only applicable when a fringe is being animated with a deformed plot. Turning this toggle
OFF will allow the fringe to animate while the deformation remains static. Needless to say, only one of these two toggles can be OFF at any one time.
Modal animation allows animations from +MAX to -MAX, whereas Ramped animation only ranges from ZERO to
+MAX of the given results values.
2D animation allows for animation frames to be created only in a 2D plane. This simply means that dynamic rotation with the mouse is not possible without recreating all the animation frames again. 3D animation allows for dynamic rotation with the mouse. The advantage of 2D over 3D animation is speed, although this is highly hardware and model size dependent. Preview will simply step through each frame and then stop. This is best used for transient animation. MPEG or VRML allows for output of animations to these standard formats, in addition to the display in the viewport. See
File>Images
(p. 197) in the MSC.Patran
Reference Manual, Part 1: Basic Functions.
Controls the window size of image output when the
MPEG or VMRL outputs are requested.Turning this toggle ON sets the output file window size to an acceptable size for most image view programs.
Enter the number of frames for the animation to build.
The default is 7. There is no currently imposed limit to the number of frames that may be used. The more frames used, the smoother the animation will appear, however practical limits such as available memory and model size will quickly dictate the limit.
The Apply button will create the plot or animation. Note that the plot or animation will occur by pressing the Apply button in either state that the form appears. In order for there to be any animation the Animate toggle must be turned ON from the Select Results form. Otherwise only a deformed or static fringe plot will appear.
2
38
PART 6
Results Postprocessing
2.4
Examples of Usage
All examples assume the Action is set to Create and the Object is set to Quick Plot.
Create only a Fringe Plot of a Scalar Result
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. Select the Fringe Result from the second listbox.
3. (Optional) If the Fringe Result contains more than one layer, select the layer using the Position button that appears below the Fringe Result listbox. The first layer will automatically be selected by default.
4. (Optional) If the Fringe Result is a vector or tensor quantity, select the scalar Quantity to be derived for the fringe. The default for tensors data is von Mises, and for vector data, is Magnitude.
5. Press the Apply button with the Animate toggle OFF.
Position...(at Z1)
Quantity: von Mises
Apply
Z
Y
X
209735.
196421.
183107.
169794.
156480.
143166.
129852.
116539.
103225.
89911.
76598.
63284.
49970.
36656.
23343.
Figure 2-1 Fringe Plot of Stresses in a Cantilever Plate.
Create only a Deformation Plot
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. Select the Deformation Result from the bottom listbox.
3. (Optional) Be sure that no Fringe Result has been selected in the Fringe Result listbox. Deselect it if one has.
4. Press the Apply button with the Animate toggle OFF.
CHAPTER 2
Quick Plots
39
2
Apply
Y
X
Figure 2-2 Deformation Plot of Cantilever Plate with
Undeformed Shape.
2
40
PART 6
Results Postprocessing
Create a Fringe on a Deformed Plot
1. From the Select Results form (left most icon) select a
Result Case from the first listbox.
2. Select a Fringe Result from the second listbox.
3. (Optional) If the Fringe Result contains more than one layer, select the layer using the Position button that appears below the Fringe Result listbox.The first layer will automatically be selected by default.
4. (Optional) If the Fringe Result is a vector or tensor quantity, select the scalar Quantity to be derived for the fringe. The default for tensors data is von Mises, and for vector data, is Magnitude.
5. Select a Deformation Result from the bottom listbox.
6. Press the Apply button with the Animate toggle OFF.
Position...(at Z1)
Quantity: von Mises
Apply
Z
Y
X
209735.
196421.
183107.
169794.
156480.
143166.
129852.
116539.
103225.
89911.
76598.
63284.
49970.
36656.
23343.
Figure 2-3 Fringe Plot on a Deformation Plot of
Cantilever Plate with Undeformed Shape.
CHAPTER 2
Quick Plots
41
Create a Maximum Fringe from Multiple Layers
1. From the Select Results form (left most icon) select a
Result Case from the first listbox.
2. Select a Fringe Result from the second listbox.
3. The Fringe Result must contain more than one layer.
Select all the layers using the Position button that appears below the Fringe Result listbox.
4. From the form that appear when selecting positions, change the Option to Maximum.
5. (Optional) If the Fringe Result is a vector or tensor quantity, select the scalar Quantity to be derived for the fringe. The default for tensors data is von Mises, and for vector data, is Magnitude.
Position...(at Z1)
Option:
Maximum
Quantity: von Mises
6. Press the Apply button with the Animate toggle OFF. A fringe plot will result by performing a maximum comparison and extraction of the selected layers for the requested scalar quantity.
Apply
Animate a Mode Shape
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. Select the Deformation Result from the bottom listbox.
3. (Optional) Be sure that no Fringe Result has been selected in the Fringe Result listbox. Deselect it if one has.
4. Turn the Animate toggle ON. Modal animations are the default.
5. Press the Apply button.
Animate
Apply
2
Z
Y
X
Figure 2-4 Modal Animation of Cantilever Plate.
2
42
PART 6
Results Postprocessing
Animate a Deformed Shape
1. Follow the previous example of
2. Turn the Animate toggle ON.
3. Press the Animation Options button icon.
4. Change the Animation Method from Modal to Ramped.
This will allow animation from ZERO to +MAX as opposed to the default -MAX to +MAX of the selected results quantities.
5. Press the Apply button.
Animate a Fringe Result and a Deformation Simultaneously
2. Turn the Animate toggle ON.
3. (Optional) Change any necessary Animation Options.
4. Press the Apply button. Both the fringe and deformation plots will animate together in a linear fashion.
Animate a Fringe Plot Only
Create only a Fringe Plot of a
(p. 38). Make sure that no deformation plot
has been requested.
2. Turn the Animate toggle ON.
3. (Optional) Change any necessary Animation Options.
4. Press the Apply button.
Animate a Deformed Plot or Mode Shape with a Static Fringe
2. Turn the Animate toggle ON.
3. Press the Animate Options icon button.
Animate
◆
Ramped
Apply
Animate
Apply
Animate
Apply
Animate
CHAPTER 2
Quick Plots
43
4. Turn the Animate Fringe toggle OFF on the Animate
Options form.
5. Press the Apply button. The fringe plot will remain static as the deformation animates.
Animate a Fringe on a Static Deformed Plot
2. Turn the Animate toggle ON.
3. Press the Animate Options icon button.
Animate Fringe
Apply
Animate
4. Turn the Animate Fringe toggle OFF on the Animate
Options form.
5. Press the Apply button. The fringe will animate on the static deformed shape of the model.
Animate Deformation
Apply
Change Display Attributes of a Deformed Plot, Fringe Plot or Animation
Follow any of the procedures described above to create a deformation or fringe plot or animation or combination thereof. But before pressing Apply do the following:
1. (Optional) Change deformation attributes by pressing the
Deform Attributes button icon.
For example, change the Line Style to Dashed for the
Undeformed geometry.
2. (Optional) Change fringe attributes by pressing the
Fringe Attributes button icon.
For example change the fringe Style to Element Fill.
3. Press the Apply button.
Apply
2
2
44
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing1
CHAPTER
3
Deformation Plots
■
■
■
■
■
3
56
PART 6
Results Postprocessing
3.1
Overview
For an overview of how the Results Application works please see
(p. 1). To specifically make or modify a deformation plot, select Create or
Modify from the Action pull-down menu on the Results application form; and select
Deformation from the Object pull-down menu.
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a new deformation plot and Modify is used to change an existing one. If you try to modify an existing plot with Create you will be asked for overwrite permission, whereas Modify assumes that the action is desired, so no overwrite permission is requested.
Toggles the form to select results for deformation plots. This is the default mode of the Deformation form.
For both Modify and Create the same basic operations and options are available. To create or modify a deformed plot the following basic steps must be followed:
1. Set the Action to Create or Modify and the Object to Deformation.
2. Select a Result Case or Cases from the Select Result Case(s) listbox.
See
(p. 16) for a detailed explanation of this
process as well as
3. Select a deformation result from the Select Deformation Result listbox.
4. At the bottom of the form, indicate whether the deformation plot is to be plotted in Resultant or individual Component form.
Individual components are indicated as XX, YY, or ZZ which for cylindrical and spherical coordinate systems translates to and
r
, ,
r
, ,
Z
, respectively. Toggle the component(s) that you don’t wish to plot OFF.
5. Optionally select the target entities, change display attributes, or invoke other plot options by changing these settings using the three middle icons at the top of the form. These are described in detail later in this chapter.
CHAPTER 3
Deformation Plots
57
6. If animation is desired, turn the Animate toggle ON in the main form where results are selected and optionally change animation options with the right most icon at the top of the screen. For
detailed explanations of animation options see
7. Press the Apply button when ready to create the deformation plot.
Apply
To modify an existing deformation plot, simply follow the above procedure with the Action set to Modify. However, you must first select an existing plot using the Existing Deformation Plots button on the main form where results are selected. When an existing deformation plot is selected, all results, attributes, and options in the various widgets associated with that plot are updated to reflect that plot’s settings. You may then proceed to modify the plot.
By default a deformation plot with the name default_Deformation
will be created unless the user specifically gives a different name. Multiple deformation plots can only be created and posted by giving separate names. Multiple deformation plots can be posted to the same viewport or to separate viewports. Each viewport can have its own set of deformation plots or other plot types posted. This is also true for animation of these plots. Only animation in the same viewport will be synchronized.
Each plot can have its own attributes. Each plot can also target or be displayed on separate entities and have its own associated options. These are detailed in the next sections.
3
3
58
PART 6
Results Postprocessing
3.2
Target Entities
Deformation plots can be displayed on various model entities. By default deformation plots are displayed using the entire model displayed in the current viewport. To change target entity selection for deformed plots on the Results Display form, set the Object to Deformation, and press the Target Entities selection button.
Toggles the form to select target display entities for deformation plots.
The following table describes which entities deformation plots can target:
Entity
Current Viewport
Nodes
Elements
Groups
Materials
Properties
Element Types
Description
By default all deformation plots are displayed on all finite element entities displayed in the currently active viewport (the entire displayed model).
Individual nodes may be selected on which to display the deformed shape. You may type in any node numbers manually or by selecting them graphically from the screen. Be sure to include the word Node in front of the IDs you type in manually, (i.e., Node 1 5 55 100 etc.). To select all nodes use the syntax “Node 1:#.”
Individual elements may be selected on which to display the deformed shape. You may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55
100 etc.). To select all elements use the syntax “Elem 1:#.”
Deformation plots can be limited to only selected groups. A listbox will appear allowing selection of the groups to which the deformation plot will be applied. This is handy in that the same finite element entities can belong to multiple groups. Only those groups selected will be displayed in a deformed condition while all other non-selected groups will remain in their undeformed shape and retain their own display attributes.
Deformation plots can be targeted at only those finite elements which have certain material properties assigned to them. A listbox will appear allowing selection of the materials for whose elements will be displayed in a deformed shape.
Deformation plots can be targeted at only those finite elements which have certain element properties assigned to them. A listbox will appear allowing selection of the properties for whose elements will be displayed in a deformed shape.
Deformation plots can be limited to only certain element types also.
CHAPTER 3
Deformation Plots
59
In addition to displaying a deformation on selected entities, you may also specify the entity attributes. These are explained in the following table:
Attribute
Elements
Nodes
Description
This is the default attribute. This simply means that deformation plots will show the nodes in their deformed positions with the element connectivity following them, thus showing a true deformed shape.
Nodes as the attribute will only display the nodes in their deformed state without the element connectivity. The nodes will be displayed as small circles for better viewing.
3
Important:
Once a target entity has been selected, it will remain the target entity for the deformation plot until the user physically changes it.
3
60
PART 6
Results Postprocessing
3.3
Display Attributes
Deformation plots can be displayed in various forms. Display attributes for deformed plots are accessible by pressing the Display Attributes selection button on the Results application form with the Object set to Deformation.
Toggles the form to change display attributes for deformation plots.
The following table describes in detail the deformation display attributes which can be modified:
Attribute
Deformed/Undeformed
Color
Render Style
Line Style
Line Width
Scale Interpretation
Scale Factor
Show Undeformed
Title Editor
Description
The deformed and undeformed plots can be colored in any of 16 distinct colors as displayed by this color selection widget. The deformed and undeformed plots can have different colors assigned to them.
Render styles are Wireframe, Free Edge, Hidden Line, and
Shaded and can be applied to both the deformed and undeformed shapes. The default is Wireframe which displays all visible finite elements. Free Edge displays only those edges that pass the feature angle setting. Hidden Line hides finite elements that are behind other. Shaded will be displayed with the selected color setting.
The styles of the lines plotted for the deformed and undeformed shapes can be set to a solid line or variations of dotted lines.
The thickness of the lines in the deformed and undeformed plots is set with this attribute setting.
The visual amount of deformation is set with this parameter. The deformation can be scaled relative to the model size (Fraction of
Model Size) or can be a truly proportional representation (True
Multiplier) of the actual values. The default is Fraction of Model
Size.
The scale factor for both the Fraction of Model Size and True
Multiplier are set in this databox. The defaults are 10% (0.1) for
Fraction of Model Size and 100% (1.0) for True Multiplier.
This is a toggle to control the display of the undeformed shape. If the toggle is ON then the undeformed shape will also be plotted along with the deformed shape. If the toggle is OFF, then no undeformed shape will be plotted. Bear in mind that only one undeformed shape can be displayed in the same viewport at the same time if they are targeted at the same entities. You may not see changes to the undeformed shape if another plot has an undeformed shape plotted also.
Selecting this button opens a form that allows the deformation
CHAPTER 3
Deformation Plots
61
Attribute Description
Show Title
Lock Title
If this toggle is ON, then a title for the deformed plot is displayed.
Otherwise no title is displayed.
If this toggle is ON, then the title for the deformed plot is not modified by results form selections. Otherwise some results form selections modify the title.
Maximum Label Display
If this toggle is ON, then the maximum value in the selected results set is displayed in the viewport. Otherwise it is not displayed. For transient results or when multiple subcases have been selected, the maximum value is the maximum encountered in all the subcases.
Label Style
Label styles may be changed such as the label color, format (fixed, integer, or exponential), and the number of significant digits.
3
Important:
Once display attributes have been selected, they will remain in effect for the deformed plot until the user physically changes them. Also changes to undeformed tool attributes may not be visible if multiple deformation plots are posted to the same viewport.
3
62
PART 6
Results Postprocessing
3.4
Plot Options
Deformation plots have various options. These options for deformed plots are accessible by pressing the Plot Options selection button on the Results application form with the Object set to
Deformation.
Toggles the form to select plot options for deformation plots.
The following table describes the deformation plot options which can be modified:
Option
Coordinate
Transformation
Scale Factor
Complex No. as
Phase
Existing
Deformation Plots
Description
Vector results to display deformed plots can be transformed into any of the following coordinate systems: any user defined local system
(CID), the projection of any CID, the MSC.Patran Global system, and the nodal (analysis) coordinate system. See
(p. 305) for a definition of each of these coordinate
systems. The default is no transformation. Resulting deformation plots should look the same no matter what coordinate system they are in as long as the resultant or all components are plotted. Where coordinate transformations play a role for deformed plots is when individual components are masked out and then transformed to another coordinate system.
An additional scale factor can be given to scale the results plot above and beyond the scale factor available in the Tool Attributes form.
This scale factor has the effect of simply scaling the results up or down by the specified amount.
If complex results exist this option will be visible and specifies how and what you would like to view from results that exist as complex numbers. The options are Magnitude, Phase, Real, Imaginary, and
Angle. It is not recommended to calculate invariants (e.g., von
Mises) from complex results because the phase is not accounted for.
Phase (this is specific to Deformation Plots, Fringe Plots, and Marker
Plots) If the user selects Phase their results will be generated in degrees.
If Phase is selected, results will be generated in degrees. This is specific to Deformation Plots, Fringe Plots, and Marker Plots.
This listbox displays all existing deformation plots. You may select one of these plots from the listbox and all settings of that plot including plot attributes, target entities, option, and selected results will be restored. This is an easy mechanism to help make many plots with the settings of an existing plot without modifying the selected plot. When the Action is set to Modify, this listbox appears under the
Select Results display of the Results application form also.
CHAPTER 3
Deformation Plots
63
Option
Save Deformation
Plot As
Description
Deformation plots can be saved by name and recalled later for graphical display. Multiple deformed plots can be saved in the database and displayed simultaneously. Be aware that when multiple deformed plots are display simultaneously there could be some display problems. These deformation plots can be posted/unposted and deleted as explained in
and
(p. 27) respectively. Once a plot has been created and
named it retains all results, attributes, target entities, and options assigned to it. If no plot name is specified a default is created called default_Deformation
. As long as no plot name is specified, the default_Deformation
will be overwritten each time a plot is created or modified.
3
Important:
Once plot options have been selected, they will remain in effect for the deformed plot until the user physically changes them.
3
64
PART 6
Results Postprocessing
3.5
Examples of Usage
The following are some typical scenarios for usage of the Deformation plot tool. These instructions assume that the Action is set to Create and the Object is set to Deformation unless otherwise specified.
Create a Simple Static Deformation Plot
1. From the Select Results form (left most icon) select a Result
Case from the first listbox. If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle OFF and then select the Result Case.
2. Select the Deformation Result from the next listbox.
3. Press the Apply button with the Animate toggle OFF.
Apply
Y
X
Figure 3-1 Deformation Plot of Cantilever Plate with Undeformed
Shape.
Animate a Mode Shape
1. From the Select Results form (left most icon) select a Result
Case from the first listbox.
2. Select the Deformation Result from the next listbox.
3. Turn the Animate toggle ON.
4. Press the Apply button. Modal animations are the default therefore it is unnecessary to change any animation options.
Animate a Static Deformation
1. From the Select Results form (left most icon) select the result case from the first listbox.
2. Select the Deformation Result from the next listbox.
3. Turn the Animate toggle ON.
4. Press the Animation Options icon button.
Animate
Apply
Animate
CHAPTER 3
Deformation Plots
65
5. Change the Animate By option pulldown menu to Ramp.
Animate by: Ramp
6. Press the Apply button.
Apply
3
Z
Y
X
Figure 3-2 Modal Animation of Cantilever Plate.
Put a Fringe on a Deformed Plot
1. Create a deformation plot as explained in this chapter and make sure it is posted to the current viewport.
2. Set the Object to Fringe.
3. Create a Fringe plot in the same viewport as the
Deformation plot but change the Display Attributes before
of fringe plot creation.
3
66
PART 6
Results Postprocessing
4. In the Display Attributes for creating Fringe plots, make sure the Show on Deformed toggle is turned ON.
5. Press the Apply button for the fringe plot with the Animate toggle OFF.
Z
Y
X
209735.
196421.
183107.
169794.
156480.
143166.
129852.
116539.
103225.
89911.
76598.
63284.
49970.
36656.
23343.
Figure 3-3 Fringe Plot on a Deformation Plot of
Cantilever Plate with Undeformed Shape.
Display a Transient Animation of a Deformed Shape
1. From the Select Results form (left most icon) select the Result Cases
(time steps) from the first listbox that you wish to include in the transient animation. You must select more than one. Use the mouse and the control key to select discontinuous selections or the shift key to select a continuous selection. You can also use the Select button when the Result Cases are being displayed in abbreviated form to filter and select the Result Cases (time steps) you want. In abbreviated form the Result Case name will only appear in the listbox as the name with the number of subcases (time steps) selected, (i.e., Load Case 1, 6 of 41 subcases).
2. Select the Deformation Result from the next listbox.
3. Turn the Animate toggle ON. (If the Animate toggle is OFF then the resulting plot will be the maximum of all selected Result Cases.)
4. Press the Animation Options icon button and then select a global variable (time) to animate by. Make any other optional modifications you want.
5. Press the Apply button. This method also works with load steps, frequency steps, or simply with multiple load cases that you may wish to animate.
Show on Deformed
Apply
Animate
Apply
CHAPTER 3
Deformation Plots
67
Mask Out Deformation Components
1. Follow the instructions for
2. Go to the Select Results mode of the form.
3. At the bottom of the Select Results form change the Show As pull down menu to Components.
Show As:
Component
4. Select or de-select the components that you wish to be used in creating the deformation plot.
5. Press the Apply button.
XX YY
Apply
ZZ
3
Z
Y
X
Z
Y
X
Figure 3-4 X and Y Component Only Deformation Plots of Cantilever Beam.
Save a Deformed Plot
1. Set up the plot for a deformation as explained in
Simple Static Deformation Plot
press the Apply button.
2. Before pressing the Apply button to create a plot or an animation, press the Options icon button.
3. Type a name in the Save Deformation Plot As databox.
Save Deformation Plot As: myDeformation
4. Then press the Apply button. The plot is now saved under a specific name which can be recalled (posted/unposted) graphically when desired.
Apply
Display Multiple Deformations in the Same Viewport
1. Set up the first deformation plot as explained in the examples above but don’t press the Apply button.
2. (Optional) You will most likely have to select target entities if each plot will consist of the same deformation results.
3
68
PART 6
Results Postprocessing
3. Save the deformed plot as explained in
4. Repeat this process for as many deformation plots necessary in the same viewport. You will most likely want to change plot attributes from plot to plot also so as to be able to see the different deformations, otherwise they will all plot on top of each other.
Z
X
Figure 3-5 Two Deformation Plots in the Same Viewport,
First Torsional Mode in Wireframe and
Second Torsional Mode in Free Edge Display with Undeformed Shape.
Display Multiple Deformations in Separate Viewports
1. Set up the first deformation plot as explained in the examples above but don’t press the Apply button.
2. (Optional) Save the deformed plot as explained in
(p. 67). If you don’t specifically save the plot then a default name
will be given for each viewport such as
default_Deformation2
,
default_Deformation3
, etc.
3. Create a new viewport (from the Viewport menu on main MSC.Patran form) and make it the active viewport. This is done by placing the cursor at the edge of the viewport and clicking with the mouse. The current viewport will have a red border around it. This is the area where you click the mouse.
4. Repeat this process for as many deformation plots as necessary but change the current viewport each time.
CHAPTER 3
Deformation Plots
69
Z
Y
X
Z
Y
X
Figure 3-6 Two Deformation Plots in Separate Viewports, 2nd Bending Model in
Wireframe and 3rd Bending in Free Edge Display.
Modify a Deformation Plot or Animation
1. Set the Action to Modify with the Object set to Deformation.
2. Select an existing deformation plot using the Existing
Deformation Plots button.
Existing Deformation Plots...
3. Change results, target entities, display attributes, plot or animation options as required.
4. Press the Apply button at any time to see the results of your modifications.
Apply
3
Z
X
Figure 3-7 Existing Deformation Plot
Modified to Display Thicker Lines with Different Undeformed
Color, Line and Render Styles.
3
70
PART 6
Results Postprocessing
Display Multiple Deformation Animations in the Current Viewport
1. First create and save the deformation plots (transient or static) as explained in
Display Multiple Deformations in the Same Viewport
(p. 67) above but do not animate them.
Do not turn ON the Animate toggle.
2. (Optional) Set the Action to Post and the Object to Plots.
Post the plots that you want to animate to the current viewport if they are not already posted.
3. Set the Action to Create and the Object to Animation. One by one, select the posted plots that you wish to animate from
Animate by: Ramp
the top listbox and modify their animation method if
Update Tool
necessary. This is done by pressing the Update Tool button.
4. Press the Apply button. See
details on this procedure.
Apply
Component Suppression with Coordinate Transformation
1. Create a deformation plot as explained in
2. On the Select Results form for Deformation plots, set the
Show As pulldown to Component.
3. Turn OFF the components that you wish to suppress.
4. Go to the Plot Options form.
Show As:
Component
XX YY ZZ
5. Set the Coordinate Transformation to CID and graphically select the coordinate system of interest.
6. Press the Apply button. Only the non-suppressed components of the deformation plot will be displayed.
In the example below (
posted of a cylindrical component. The coordinate components of the global rectangular system are suppressed in adjacent plots. Finally a coordinate system transformation is performed to a cylindrical system with coordinate suppression.
CID
Apply
CHAPTER 3
Deformation Plots
71
Z
Total Deformation (all components)
X-Deformation (global rectangular)
3
Y-Deformation (global rectangular)
Z-Deformation (rectangular & cylindrical)
R-Deformation (cylindrical)
θ
-Deformation (cylindrical)
Figure 3-8 Coordinate Suppression of Deformation Plots with Coordinate Transformation into Cylindrical System.
3
72
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
4
Fringe Plots
■
■
■
■
■
4
74
PART 6
Results Postprocessing
4.1
Overview
For an overview of how the Results Application works please see
(p. 1). To specifically make or modify a fringe plot select Create or Modify from
the Action pull-down menu on the Results application form; and select Fringe from the Object pull-down menu.
A fringe plot is like a contour plot where wide color bands each representing a range of results values are plotted onto the finite element model. They differ from contour plots in that no control over the width of the color band is allowed. The color bands cover the entire finite element model.
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a new fringe plot and Modify is used to change an existing one. If you try to modify an existing plot with Create you will be asked for overwrite permission whereas
Modify assumes that the action is desired, so no overwrite permission is requested.
Toggles the form to select results for fringe plots. This is the default mode of the Fringe form.
For both Modify and Create the same basic operations and options are available. To create or modify a fringe plot the following basic steps must be followed:
1. Set the Action to Create or Modify and the Object to Fringe.
2. Select a Result Case or Cases from the Select Results Case(s) listbox.
See
(p. 16) for a detailed explanation of this
process as well as
3. Select a fringe result from the Select Fringe Result listbox.
4. If more than one layer is associated with the results, select the layer
(using the Position button) you wish to plot. These can be top or bottom results of shell elements, beam locations or laminate layers.
5. Optionally change the result Quantity. This is only possible if the selected result allows for this. If a tensor or vector result has been selected, it must be resolved to a scalar value. The various resolutions are:
CHAPTER 4
Fringe Plots
75
6. Optionally select the target entities, change display attributes, or invoke other plot options by changing these settings using the three middle button icons at the top of the form. These are described in detail later in this chapter.
7. If animations are desired, turn the Animate button ON in the main form where results are selected and optionally change animation attributes with the right most icon at the top of the screen. For detailed explanations of animation options see
8. Press the Apply button when ready to create the fringe plot.
Apply
To modify an existing fringe plot, simply follow the above procedure with the Action set to
Modify. However, you must first select an existing plot using the Existing Fringe Plots button on the main form where results are selected. When an existing fringe plot is selected, all results, attributes, and options in the various widgets associated with that plot are updated to reflect that plot’s settings. You may then proceed to modify the plot.
By default a fringe plot with the name default_Fringe
will be created unless the user specifically gives a different name. Multiple fringe plots can only be created and posted by giving separate names. Multiple fringe plots can be posted to the same viewport or to separate viewports. Each viewport can have its own set of fringe plots or other plot types posted. This is also true for animation of these plots. Only animation in the same viewport will be synchronized.
Each plot can have its own attributes. Each plot can also target or be displayed on separate entities and have its own associated options. These are detailed in the next sections.
4
4
76
PART 6
Results Postprocessing
4.2
Target Entities
Fringe plots can be displayed on various model entities. By default fringe plots are displayed on all free faces of everything displayed in the current viewport. To change target entity selection for fringe plots, press the Target Entities selection button with the Object set to Fringe.
Toggles the form to select target display entities for fringe plots.
The following table describes in detail to which entities fringe plots can be targeted. Fringe plots can only be plotted onto elements or surfaces of elements.
Entity
Current
Viewport
Elements
Groups
Materials
Properties
Element Types
Description
By default fringe plots are displayed on all finite element entities displayed in the currently active viewport. The only exception to this is when layered results exist and are associated to only certain element types. Then only those elements will display the fringe plot.
Individual elements may be selected on which to display the fringe plot.
You may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.). To select all elements use the syntax “Elem 1:#.”
Fringe plots can be limited to only selected groups. A selected group or groups must have elements in them otherwise the plot will not appear. A listbox allows selection of the group(s) to which the fringe plot will be applied. This is handy in that the same finite element entities can belong to multiple groups. Only those groups selected will be displayed with a fringe plot while all other non-selected groups will remain unaffected and retain their own display attributes.
Fringe plots can be targeted at only those finite elements which have certain material properties assigned to them. A listbox appears allowing selection of the materials for whose elements will be targeted for a fringe display.
Fringe plots can be targeted at only those finite elements which have certain element properties assigned to them. A listbox appears allowing selection of the properties for whose elements will be targeted for a fringe display.
Fringe plots can be limited to only certain element types also.
CHAPTER 4
Fringe Plots
77
In addition to targeting the above entities for a fringe plot, the fringe plot can be isolated to attributes of the entities as described in the following table:
Attribute
Free Faces
Faces
Free Edges
Edges
Target
Deformations
Description
By default all free faces of the target entities will display the fringe plot.
The fringe display will be plotted on all faces of every element for the target entities.
This will display a fringe plot on the edges that only have one common element. This results in a 1D line or edge type fringe as opposed to a 2D surface display and will generally give you the outline of your model.
This will display a fringe plot on all the edges of every element. This results in a 1D wireframe fringe type plot as opposed to a 2D surface display.
By default, fringe plots that are to be displayed on the deformed shape will be displayed on all deformation plots posted. You can select which deformation plots to target the fringe plot to by selecting deformation plots form this listbox. This listbox will only appear when more than one deformation plot exists and is posted.
4
Important:
Once a target entity has been selected, it will remain the target entity for the fringe plot until the user physically changes it.
4
78
PART 6
Results Postprocessing
4.3
Display Attributes
Fringe plots can be displayed in various forms. Display attributes for fringe plots are accessible by pressing the Display Attributes selection button on the Results application form with the
Object set to Fringe.
Toggles the form to change display attributes for fringe plots.
The following table describes in detail the fringe display attributes which can be modified:
Attribute Description
Show Spectrum
Spectrum
Range
Style
Shading
This toggle will remove or display the spectrum bar on the right of the current viewport. If the spectrum does not disappear from the graphics screen when the toggle is OFF, make sure other plots also do not have the spectrum turned ON.
This button will bring up the Spectrums form from which you can set the spectrum for the current viewport or create new spectrums.
This form operates independently of the Results application.
Therefore you do not need to press the Apply button in the Results application to effect changes in the spectrum. To learn more about changing the spectrum see
Display>Spectrums
(p. 306) in the
MSC.Patran Reference Manual, Part 1: Basic Functions.
This button will bring up a subordinate form for reassigning the range to the current spectrum in the current viewport. See
(p. 29) for details. Also from this form
you can invoke the Ranges form for creating and modifying new ranges. To learn more about changing ranges see
Display>Ranges
(p. 307) in the MSC.Patran Reference Manual, Part 1: Basic Functions.
Four fringe styles are available. The default is a Discrete/Smooth plot which will give distinct color bands which begin and end sharply. Continuous style will blend the colors together giving a smoother transition between color bands but no distinctive beginning or end to any particular color band. The Element Fill style will simply color code each element. Discrete/Flat is similar to Discrete/Smooth but may give a better or worse image depending on the graphics device.
On true color machines, fringe plots may be shaded. On machines that do not support true color, a shaded fringe plot will not look good at all. Best results are with Hardware Rendering on true color machines.
Element Shrink Factor
You can display a fringe plot with the elements shrunk a certain percentage. It is best to experiment with this.
Fringe Edges
The edge color display of the fringe plot can be changed as desired.
CHAPTER 4
Fringe Plots
79
Attribute Description
Display (Edges)
Style (Edges)
The edge display is simply the display of the finite element mesh or the display of the free edges of the model. You can choose to display either of these or none at all.
The styles of the edge lines plotted on the target entities can be set to a solid line, or variations of dotted lines.
Width (Edges)
Title Editor
Show Title
Lock Title
Show on Deformed
The thickness of the edge lines on the target entities is set with this attribute setting.
Selecting this button opens a form that allows the fringe plot title to be edited. See
If this toggle is ON, then a title for the fringe plot is displayed.
Otherwise no title is displayed.
If this toggle is ON, then the title for the fringe plot is not modified by results form selections. Otherwise some results form selections modify the title.
Show Max/Min Label
If this toggle is ON, then the maximum and minimum values of the selected results set are displayed in the viewport. Otherwise they are not displayed.
Show Fringe Label
If this toggle is ON, then the fringe label will be displayed.
Label Style
You can change the style of the numbers displayed on the spectrum bar and labels from the subordinate form that appears when you press this button. Styles can be integer, fixed, or exponential with specification of the number of significant digits.
The fringe plot will be displayed on the deformed shape of the model if a deformation plot has also been posted the current viewport. The fringe plot will display on all deformation plots if more than one is posted to the viewport by default. If this is not desired, see
4
Important:
Once display attributes have been selected, they will remain in effect for the fringe plot until the user physically changes them.
4
80
PART 6
Results Postprocessing
4.4
Plot Options
Fringe plots have various options. Plot options for fringe plots are accessible by pressing the Plot
Options selection button.
Toggles the form to select plot options for fringe plots.
The following table describes in detail the fringe plot options which can be modified:
Option
Coordinate
Transformation
Scale Factor
Filter Values
Averaging Domain
Description
Vector and tensor results to display fringe plots can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the MSC.Patran global system, a material coordinate system, element IJK coordinate system or the nodal (analysis) coordinate system depending on the type of result (vector, or tensor). See
definition of each of these coordinate systems. The default is no transformation, which will plot data in the coordinate frame as stored in the database. Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user.
These can vary from node to node. Element data can be stored from the analysis code in any coordinate system. Note also that the analysis translators that import the results data into the database can transform results. Check with the appropriate translator guide.
This scale factor has the effect of simply scaling the results up or down by the specified amount. This will have an effect on the fringe plot but will not effect the spectrum range values.
By specifying a filter value, a gate will be used to keep values below a maximum, above a minimum, between a certain range, or at the exclusion of certain values. The default is none. If filtering is used, only those elements which pass the filter gate will display a fringe plot on them. In other words, the fringe plot will not be displayed on elements that don’t pass the filter test completely.
For element based result quantities that must be displayed at nodes, an averaging domain must be used since more than one result will exist for each node. There is a contribution from each element attached to any particular node. By default all entities which contribute are used. Alternatively, you can tell the Results application to only average results from those elements that share the same material or element property, are from the same target entities, or have the same element type. For more details, see
CHAPTER 4
Fringe Plots
81
Option Description
Averaging Method
Extrapolation
Method
Complex No. as
The method in which certain results are determined can make a difference to the actual displayed plot. This is important when derived results from element based tensor or vector results are used such as von Mises stress or Magnitude displacements, For instance, if you average at the nodes first and then derive the desired quantity, you may get a different answer than if you derive first and then average. It is left up to the user to decide which is correct. For more
Many times, element based results that are to be displayed at nodes exist at locations other than the nodes such as at integration points.
Various methods are available to the user to extrapolate these results out to the nodes. For more details, see
The Real component of a complex number is the default by which results will be postprocessed. To force the postprocessor to use a different quantity such as Magnitude, Imaginary, Phase, or Angle, set this option pull down menu. This option will only be available if a complex result has been selected. It is not recommended to calculate invariants (e.g., von Mises) from complex results because the phase is not accounted for.
Use PCL Expression
The results can be modified with a user defined PCL expression.
Define PCL
Expression
Existing Fringe
Plots
This listbox displays all existing fringe plots. You may select one of these plots from the listbox and all settings of that plot including display attributes, target entities, option, and selected results will be restored. This is an easy mechanism to help make many plots with the settings of an existing plot without modifying the selected plot.
When the Action is set to Modify, this listbox appears under the
Select Results display of the Results application form also.
Save Fringe Plot As
Fringe plots can be saved by name and recalled later for graphical display. Multiple fringe plots can be saved in the database and displayed simultaneously. Be aware that when multiple fringe plots are displayed simultaneously there could be some display problems if they are displayed on the same entities. These fringe plots can be
posted/unposted and deleted as explained in
and
(p. 27) respectively. Once a plot has been created and
named it retains all results, attributes, target entities, and options assigned to it. If no plot name is specified a default is created called default_Fringe
. As long as no plot name is specified, the default_Fringe
will be overwritten each time a plot is created or modified.
4
Important:
Once plot options have been selected, they will remain in effect for the fringe plot until the user physically changes them.
4
82
PART 6
Results Postprocessing
4.5
Examples of Usage
The following are some typical scenarios for usage of the Fringe plot tool. These instructions assume that the Action is set to Create and the Object is set to Fringe unless otherwise specified.
Create a Simple Static Fringe Plot
1. From the Select Results form (left most icon) select the
Result Case from the first listbox. If more than one subcase exists for a Result Case, turn the Abbreviate
Subcases toggle OFF and then select the Result Case.
2. Select the Fringe Result from the next listbox.
3. (Optional) If the selected result has more than one layer associated with it, select the layer using the layer Position button.
Position...(at Z1)
4. (Optional) If the result is a vector or tensor, select a resolved scalar results value from the results Quantity pull-down menu (such as von Mises stress or Magnitude displacement).
Quantity: von Mises
5. Press the Apply button with the Animate toggle OFF.
Apply
Z
Y
X
209735.
196421.
183107.
169794.
156480.
143166.
129852.
116539.
103225.
89911.
76598.
63284.
49970.
36656.
23343.
Figure 4-1 Fringe Plot of von Mises Stress on Cantilever Plate.
CHAPTER 4
Fringe Plots
83
Animate a Static Fringe Plot
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. Select the Fringe Result from the next listbox.
3. (Optional) If the selected result has more than one layer associated with it, select the layer using the result Position button.
Position...(at Z1)
4. (Optional) If the result is a vector or tensor, select a resolved
Quantity:
scalar results value from the results Quantity pull-down menu (such as von Mises stress or Magnitude displacement).
von Mises
5. Turn the Animate toggle ON.
Animate
6. Press the Animation Options icon button.
7. Change the Animate By option pulldown menu to Ramp.
Animate by: Ramp
8. Press the Apply button.
Apply
4
4
84
PART 6
Results Postprocessing
Put a Fringe on a Deformed Plot
1. Create a deformation plot and make sure it is posted to the
explanation of deformation plot creation.
2. Now make a fringe plot as explained in
(p. 82), but do not press the Apply
button.
3. Press the Display Attributes icon button.
4. Turn ON the Show on Deformed toggle.
5. (Optional) If more than one deformation plot exists and is posted to the viewport, you can optionally specify on which deformation plots to display the fringe plot. This is done under the Target Entities option. Otherwise the Fringe plot will show on all Deformation plots posted.
6. Press the Apply button with the Animate toggle OFF.
Z
Y
X
209735.
196421.
183107.
169794.
156480.
143166.
129852.
116539.
103225.
89911.
76598.
63284.
49970.
36656.
23343.
Figure 4-2 Fringe Plot of von Mises Stress on Deformed Cantilever Plate.
Show on Deformed
Apply
CHAPTER 4
Fringe Plots
85
Display a Transient Fringe Animation
1. From the Select Results form (left most icon) select the
Result Cases (time steps) from the first listbox that you wish to include in the transient animation. You must select more than one. Use the mouse and the control key to select discontinuous selections or the shift key to select continuous selection. You can also use the Select button when the Result Cases are being displayed in abbreviated form to filter and select the subcases (time steps) you want.
In abbreviated form the Result Case name will only appear in the listbox as the name with number of subcases (time steps) selected, (i.e., Load Case 1, 6 of 41 subcases).
2. Select the Fringe Result from the next listbox.
3. (Optional) If the selected result has more than one layer associated with it, select the layer from the result Position pull-down menu.
Position...(at Z1)
4. (Optional) If the result is a vector or tensor, select a resolved
Quantity: von Mises
scalar results value from the results Quantity pulldown menu (such as von Mises stress or Magnitude displacement).
5. Turn the Animate toggle ON. (If the Animate toggle is OFF then the resulting plot will simply plot up a maximum plot of all selected Result Cases and will not animate.)
6. Press the Animation Options icon button.
Animate
7. Select a Global Variable (time) to Animate By. Make any other optional modifications you want.
8. Press the Apply button. This method also works with load steps, frequency steps, or simply with multiple load cases that you may wish to animate.
Animate by: Global Variable
Apply
4
Z
Y
X
Figure 4-3 Exaggerated Transient Animation of Displacements with Fringe Superimposed on Deformed Shape.
4
86
PART 6
Results Postprocessing
Save a Fringe Plot
1. Set up the fringe plot as explained in
(p. 82) but do not press the Apply button.
2. Before pressing the Apply button to create a plot or animation, press the Plot Options icon button.
3. Type a name in the Save Fringe Plot As databox.
Save Fringe Plot As: myFringe
4. Then press the Apply button. The plot is now saved under a specific name which can be recalled (posted/unposted) graphically when desired.
Apply
Display Multiple Fringe Plots in the Current Viewport
1. Set up the first fringe plot as explained in the previous examples, but do not press the Apply button.
2. (Optional) You will most likely have to select target entities so as not to overlap fringe plots.
3. Save the fringe plot as explained in
4. Repeat this process for as many fringe plots as necessary.
To put up multiple fringe plots in different viewports, simply make the viewport of interest active by clicking the mouse in its border and following the same procedure. An active viewport has a red border around the graphics.
Z
Y
X
Figure 4-4 Two Fringe Plots Targeting Certain Elements,
One on the Undeformed Shape and One on the Deformed Shape.
Modify a Fringe Plot or Animation
1. Set the Action to Modify with the Object set to Fringe.
2. Select an existing fringe plot using the Existing Fringe Plots button.
Existing Fringe Plots...
3. Change results, target entities, display attributes, plot or animation options as required.
4. Press the Apply button at any time to see the results of your modifications.
Apply
CHAPTER 4
Fringe Plots
87
Display Multiple Animations in the Current Viewport
1. First create and save the fringe plots (transient or static) as explained in
Display Multiple Fringe Plots in the Current
(p. 86), but do not animate them. Do not turn ON
the Animate toggle.
2. (Optional) Set the Action to Post and the Object to Plots.
Post the plots to the viewports that you want if they are not already posted. They can be any plot type that supports animation.
3. Set the Action to Create and the Object to Animation. One by one, select the posted plots that you wish to animate from
Animate by: Ramp
the top listbox and modify their animation method if necessary. This is done by pressing the Update Tool button.
Update Tool
4. Press the Apply button. See
details on this method.
Apply
4
4
88
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
5
Contour Line Plots
■
■
■
■
■
4
90
PART 6
Results Postprocessing
5.1
Overview
For an overview of how the Results Application works, please see
(p. 1). To specifically make or modify a contour line plot, select Create or
Modify from the Action pull-down menu on the Results application form and select Contour from the Object pull-down menu.
The lines rendered in a contour line plot show the locations within the model where a specific result value exists. Contour line plots can be rendered with and without labels. Characters (e.g. a, b, c, etc.) are used for the contour line labels. When labeling is turned off, you must use the contour line color to determine the numerical value each line represents by matching the color with the viewport’s spectrum range. Since there can be only one spectrum for all plots shown within a Patran viewport, you will see that the contour line values are indicated with characters placed at the mid-location of the spectrum’s numerical intervals. The contour line value is the average of its interval’s maximum and minimum range values. If a Fringe plot is also shown in the viewport, its color bands relate to the range of values represented by each color band.
Only the two options, Create and Modify, exist for the Action method of the tool. The functional difference between these is as follows. Create must be used to derive a new contour plot whereas
Modify is used to change an attribute of an existing contour plot. If you choose to Modify an existing plot, you can identify the existing plot by pressing the Existing Contour Plot button on the top of the form.
After you set the Action to either Create or Modify you will need to perform the following steps to completely define your contour plot.:
1. Select a Result Case or Cases from the Select Results Case(s) listbox.
See
detailed description of this step.
2. Next, select a contour result type from the Select Contour Result listbox.
3. If the result is associated to positions within your simulation model
(e.g. layer, shell, or beam section positions), you should select the
Position button and specify the position for the result type.
4. A result Quantity can be optionally selected. This will cause Patran to calculate this quantity from the result type you have selected in step 2 above.
CHAPTER 5
Contour Line Plots
91
5. After performing steps 1-4 you have now defined the numerical value the contour plot will represent. To specify which portion of the model plot will be rendered (i.e. plot target), its graphical display attributes, or to further specify various numerical operations that you would like to apply to the result data you will need to select the second through fourth icons respectively.
6. If a contour animation is desired, select the Animate button. For a detailed description of the animation options, see
7. Press the Apply button when you are ready to create the contour plot.
Apply
When creating a contour plot you can specify its name so you can define multiple contour plots with varying definitions. The plot name is entered within the Plot Options sub form (i.e. the fourth icon described in step 5). If you do not specify a name the default name, default_contour, will be used. Multiple contour plots can only be created and posted by defining separate names. Multiple contour plots can be posted to the same viewport or to separate viewports. Each viewport can have multiple plot types posted within it.
The following sections discuss in detail the various options that are found in the plot sub forms that correspond to the steps shown above.
4
4
92
PART 6
Results Postprocessing
5.2
Target Entities
Contour plots can be displayed on various model entities. By default, Contour plots are displayed on all free faces of all elements displayed in the current viewport. To change the target entity selection for your Contour plot, press the Target Entities selection button with the Object set to Contour.
Toggles the form to select target display entities for Contour plots.
The following table describes in detail to which entities Contour plots can be targeted upon.
Contour plots can only be rendered on element entities.
Entity
Current
Viewport
Elements
Groups
Materials
Properties
Element Types
Description
By default, Contour plots are displayed on all finite element entities displayed within the current viewport.
Individual elements may be selected for the Contour plot. You may enter the element ids manually or select them graphically. Be sure to include the word Elem in front of the ids you enter (e.g. Elem 1, 5, 55, 100:102 etc.). To select all elements use the following syntax. “Elem 1:#.”
Contour plots can be rendered on selected groups. The selected group(s) must contain elements.
Contour plots can be rendered upon finite elements which have a specific associated material type.
Contour plots can be rendered upon finite elements which have a specific associated element property set.
Contour plots can be rendered upon specific element types (e.g. Quad4,
Hex8, etc.).
CHAPTER 5
Contour Line Plots
93
5.3
Display Attributes
The graphical elements of a Contour plot can be modified by changing its various display attributes. Display attributes for Contour plots are accessed by pressing the Display Attributes selection icon.
Toggles the form to show the available display attributes for the Contour plot.
The following table describes the Contour display attributes which can be modified:
Attribute Description
Spectrum / Constant
The radio buttons, Spectrum and Constant, allow you display contour lines with either a spectrum of colors relative to their numerical value or as a single color respectively.
Show Spectrum
Show Viewport
Legend
This toggle will remove or display the spectrum bar within the current viewport. If you set the toggle off and spectrum is still displayed, check if you have other plots posted in the viewport. If there are other plots, you will need to set this toggle off for all plots posted in the viewport.
This toggle will remove or display the legend that is shown in the lower right hand corner of the viewport. This legend displays the plot name and which entity contains the maximum and minimum result values. If you set the toggle off and the legend is still displayed, check if you have other plots posted in the viewport. If there are other plots, you will need to set this toggle off for all plots posted in the viewport.
Spectrum
Range
This button will activate the Spectrum form. This form allows you to select an existing spectrum to be associated to the current viewport. It also allows you to define a new spectrum. Since this form is independent of the Results application, you will not need to press the Apply button on the Results application to effect changes to the spectrum. To learn more about changing the
(p. 90) of the MSC.Patran Reference Manual,
Part 6: Results Postprocessing.
This button will activate the Range sub form. This form allows you to assign an existing range to the viewport’s spectrum. See
(p. 29) for details. The form also allows
you to modify an existing range or create a new range. To learn
Reference Manual, Part 6: Results Postprocessing.
Element Edges
This button allows you to change the color that the element edges are rendered with.
Display
(Element Edges
)
This pop down button allows you to select which element edges are rendered. The selection includes Free Edges and Element
Edges which cause either the elements free edges or all element edges to be rendered respectively.
4
4
94
PART 6
Results Postprocessing
Attribute Description
Style
(Element Edges
Width
Contour Style
Contour Width
Title Editor
)
(Element Edges
)
The Style pop down button allows you to control the line type that is used to render the element edges. The selections are solid, dashed, dotted, and dot-dash line styles.
This pop down button allows you to control the thickness of the rendered element edges.
The Contour Style pop down button allows you to control the line type that is used to render the contour lines. The selections are solid, dashed, dotted, and dot-dash line styles.
This pop down button allows you to control thickness of the contour lines.
Selecting this button opens a form that allows the contour plot title to be edited. See
Show Title
Lock Title
If this toggle is ON, then a title for the contour plot is displayed.
Otherwise no title is displayed.
If this toggle is ON, then the title for the contour plot is not modified by results form selections. Otherwise some results form selections modify the title.
Show Max/Min Label
If this toggle is ON, the maximum and minimum value of the selected result type will be displayed. Their value labels will be rendered in a color different than all other value labels.
Label Frequency
As you adjust the Label Frequency slider from 0 to Max the spacing between the contour line labels will decrease therefore increasing the label density. To turn off contour labeling adjust the slider to zero. Zero label frequency is the default frequency value.
Label Style
Show on Deformed
Pressing the Label Style button causes the Contour Label Style form to appear. The form allows you to modify the label color, format (e.g. fixed, exponential, and integer), and significant figures of the plot’s range and maximum/minimum labels.
If this toggle is set ON, the Contour plot will be targeted on the model’s posted deformed shape. By default, the Contour plot will display on all deformation plots posted in viewport. If this is not desired, see
CHAPTER 5
Contour Line Plots
95
5.4
Plot Options
The Plot Options form includes numerical operations that can be applied to the result type you chose previously in the Select Results form. The options that appear on this form are relative to the selected result type’s data type (i.e. scalar, vector, or tensor). The following table describes the various operations that can be applied.
Toggles the form to select numerical plot options for Contour plots.
Option
Coordinate
Transformation
Scale Factor
Filter Values
Averaging Domain
Averaging Method
Extrapolation
Method
Description
Vector and tensor results can be transformed into any of the following coordinate systems. The AsIs coordinate system, any user defined local system (CID), the projection of any CID, the
MSC.Patran global system, material, element IJK, or the default
description of each coordinate system type. AsIs is the default option.
The scale factor is a numerical multiplier that is applied to the data after all other numerical operations have transformed the raw analysis data to its final form.
By specifying a filter value, you can create a gate that will be used to include values below a maximum, above a minimum, between a certain range, or exclude a range of values. The default option is none. If filtering is used, contour lines will only be rendered on elements that contain values allowed by the filter.
For element based result quantities that must be displayed at node locations an Averaging Domain must be specified. As the element’s analysis result is moved to the element’s node locations multiple values can occur at nodes that are shared by adjacent elements. The
Averaging Domain options describe to Patran which of the multiple result values you want to resolved to a single value. For more
The Averaging Method describes to Patran the order of operations that will be applied to the selected results data and the operation type that will be used to resolve multiple values to a single value at the model’s node locations. For example, the Derive/Average option will cause the user specified quantity derivation (e.g.
Principal stress, extract the x-component of translational displacement) to occur first, before a simple average is applied to resolve multiple results that occur at the shared element’s node
locations. For more details see
Many times, element based results must be moved from their initial element location to another location (e.g. element integration points to element node locations). The Extrapolation Method defines which algorithm will be used for this operation. For more details, see
4
4
96
PART 6
Results Postprocessing
Option Description
Complex No. as
If the result value you have chosen to post process is complex, then an option button will appear that allows you to show the results real, complex, magnitude, or phase representation.
Use PCL Expression
This toggle button will activate the Define PCL Expression button
Define PCL
Expression
The sub form that will appear when you press this button will allow you to further modify the selected result data by applying a user
defined PCL expression. For more details, see
Existing Contour
Plots
Save Contour Plot
As
This listbox displays all existing Contour plots. If you select an existing plot from the listbox, the plot’s definition will be used to define each sub formsub form’s various options.
Contour plots can be saved by name and recalled later for editing.
Saved Contour plots can be posted, unposted and deleted as shown
(p. 27) respectively. Once a plot
has been named, its definition is automatically persisted in the
Patran database when you hit the Apply button to create the plot.
CHAPTER 5
Contour Line Plots
97
5.5
Contour Plot Example
The following is an example of creating a contour plot superimposed on a deformed shape plot.
Create a Contour Plot
1. After setting the Action/Object/Method to
Create/Contour/Lines, select a Result Case from the
Select Result Case(s) list box.
2. Next, select the Stress Tensor result type from the Select
2DContour Result list box.
3. (Optional) If the selected result has more than one layer associated with it select the layer using the layer Position button.
4. Select the Y Component from the Quantity pull down option menu.
5. Press the Apply button with the Animate toggle OFF to create the plot.
Position...(at Z2)
Quantity: Y Component
Apply
4
Figure 5-1 Contour Plot of the Y-Component of Stress on Cantilever Plate.
4
98
PART 6
Results Postprocessing
Create a Contour on a Deformed Plot
1. Create a deformation plot and make sure it is posted to the
explanation of deformation plot creation.
2. Now create a Contour plot as explained in
(p. 97), but do not press the Apply button.
3. Press the Display Attributes icon button.
4. Turn ON the Show on Deformed toggle.
5. Press the Apply button with the Animate toggle OFF.
Show on Deformed
Apply
Figure 5-2 Contour Plot of the Y-Component of Stress on Deformed Cantilever Plate.
CHAPTER 5
Contour Line Plots
99
Create a Contour plot with contour labels on a Deformed Plot
1. Similar the previous example, create a deformation plot and make sure it is posted to the current viewport. See
deformation plot creation.
2. Next, create a Contour plot as explained in
(p. 97), but do not press the Apply button.
3. Press the Display Attributes icon button.
4. Slide the Label Frequency to the right until a frequency of
10 is achieved.
5. Turn ON the Show on Deformed toggle.
6. Press the Apply button with the Animate toggle OFF.
Show on Deformed
Apply
4
Figure 5-3 Contour Plot of the Y-Component of Stress on Deformed Cantilever Plate.
4
100
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
6
Marker Plots
■
■
■
■
■
5
102
PART 6
Results Postprocessing
6.1
Overview
Marker plots are scalar, vector and tensor plots. For an overview of how the Results Application works please see
Introduction to Results Postprocessing
(p. 1). To specifically make or modify a marker plot select Create or Modify from the Action pull-down menu on the Results
Display form; and select Marker from the Object pull-down menu. Then set the marker type to
Scalar, Vector, or Tensor from the Method pull-down menu.
Selecting Results
(p. 16)
Scalar plots are scalable colored markers of various forms, e.g. triangles, squares, diamonds which represent the selected scalar result quantities displayed at nodes and elements.
Vector plots are similar to deformation plots except that instead the representation of the results is displayed as three arrow (vectors) at right angles to one another representing each coordinate contribution. The component vectors can also be resolved into a resultant vector. Any deformation plot can also be represented as a vector plot. There are of course other applications for vector plots such as viewing principal stresses.
Tensor results are similar to vector results except they have six components associated with them (the upper triangular portion of a 3x3 matrix). Typically results for tensor plots are component stress.
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a new marker plot and Modify is used to change an existing one. If you try to modify an existing plot with Create you will be asked for overwrite permission whereas
Modify assumes that the action is desired, so no overwrite permission is requested.
Toggles the form to select results for marker plots. This is the default mode of the Marker plot form.
CHAPTER 6
Marker Plots
103
For both Modify and Create the same basic operations and options are available. To create or modify a marker plot the following basic steps must be followed after setting the marker type
(Scalar, Vector, or Tensor):
1. Set the Action to Create or Modify, the Object to Marker and the
Method to Scalar, Vector, or Tensor.
2. Select a Result Case or Cases from the Select Results Case(s) listbox.
See
Selecting Results
(p. 16) for a detailed explanation of this process as well as
Filtering Results
(p. 19).
3. Select a result from the Select Scalar/Vector/Tensor Result listbox.
4. If more than one layer is associated with the results, select the layer
(using the Position button) you wish to plot. These can be top or bottom results of shell elements, beam locations or laminate layers.
5. Optionally change the result Quantity. This is only possible if the selected result allows for this. If either a tensor or vector result is selected for a scalar marker plot then it must be resolved to a scalar value. If a tensor result has been selected for a vector marker plot, it must be resolved to a vector value. The various resolutions are:
Tensor to Scalar
von Mises, X, Y, Z, XY, YZ, ZX, XY
Engineering, ZX Engineering, ZX
Engineering, Maximum Principal, Minimum
Principal, Middle Principal, Hydrostatic, 1st
Invariant, 2nd Invariant, 3rd Invariant,
Tresca, Maximum Shear, Octahedral,
Maximum Principal 2D, Minimum Principal
2D, Tresca 2D, Maximum Shear 2D.
Vector to Scalar
Magnitude, X, Y or Z Component.
Tensor to Vector:
Minimum Principal, Middle (intermediate)
Principal, Maximum Principal, Component,
Minimum Principal 2D, Maximum Principal
2D.
6. Optionally, for tensor or vector marker plots, change the form in which to display the tensor or vector: as components, resultants or principal values. This is done in the Show As pull-down menu at the bottom of the main Select Results form.
7. Optionally select the target entities, change display attributes, or invoke other plot options by changing these settings using the three middle icons at the top of the form. These are described in detail later in this chapter.
8. If animations are desired, turn the Animate button ON in the main form where results are selected and optionally change animation attributes with the right most icon at the top of the screen. For detailed explanations of animation options see
9. Press the Apply button when ready to create the marker plot.
Apply
5
5
104
PART 6
Results Postprocessing
To modify an existing marker plot, simply follow the above procedure with the Action set to
Modify. However, you must first select an existing plot using the Existing Scalar/Vector/Tensor
Plots button on the main form where results are selected. When an existing marker plot is selected, all results, attributes, and options in the various widgets associated with that plot are updated to reflect that plot’s settings. You may then proceed to modify the plot.
By default a marker plot with the name default_Scalar, default_Vector or default_Tensor will be created unless the user specifically gives a different name. Multiple marker plots can only be created and posted by giving separate names. Multiple marker plots can be posted to the same viewport or to separate viewports. Each viewport can have its own set of marker plots or other plot types posted. This is also true for animation of these plots. Only animation in the same viewport will be synchronized.
Each plot can have its own attributes. Each plot can also target or be displayed on separate entities and have its own associated options. These are detailed in the next sections.
Component selection is represented as XX, YY, and ZZ for the three component directions of any coordinate system. These translate into
r
, ,
z
and
r
φ θ
for cylindrical and spherical coordinate systems respectively.
Tensor Notes.
By default tensors are displayed as vectors without arrow heads, each with its own color code and result label (value). Traditional tensors with a box and vectors with arrow heads can also be created by changing display attributes. For two dimensional tensors, the default plots are know as “Crow’s Feet” and display two axial and one shear (coupled) component or the two principals (maximum and minimum). This display is supported for running loads, moments, stresses, and strains. The results can be rotated to any direction desired.
The tensor results for element strains are displayed at the mid-plane and outer fiber locations in two different manners.
1. Three legged tensor display indicating axial and shear directions with the appropriate result quantities labeled at the ends of the tensor.
2. From one to n number of axial strain values in directions relative to the requested orientation.
For anisotropic elements, the strain tensor directions will default to
, , ±
45
°
. For elements that reference a laminate, the default strain tensor directions will be 0, 90 and those directions corresponding to each lamina’s orientation. The default angles can be modified and additional angles can be specified. The principal results can also be displayed as principal components at the element centroid with the same axes display.
Tensors can also be treated as two dimensional or three dimensional. The default is three dimensional, however the generic method will look at the data to determine whether to use the
2D or the 3D calculations. The 2D calculation method will ignore the YY, ZZ, and ZX components. The 3D method will treat zero component values as significant.
CHAPTER 6
Marker Plots
105
6.2
Target Entities
Marker plots can be displayed on various model entities. By default marker plots are displayed on all nodes displayed in the current viewport regardless of the results data type (elemental or nodal based). To change target entity selection for marker plots, press the Target Entities selection button with the Object set to Marker and the appropriate Method (Scalar, Vector, or
Tensor) selected.
Toggles the form to select target display entities for marker plots.
The following table describes in detail which entities marker plots can be targeted.
Entity Description
Current
Viewport
Nodes
Elements
Groups
Materials
By default all marker plots are displayed on all finite element nodes displayed in the currently active viewport. Elemental based results are extrapolated out to the nodes and averaged.
Individual nodes may be selected on which to display the marker plot.
You may type in any node numbers manually or by selecting them graphically from the screen. Be sure to include the word Node in front of the IDs you type in manually, (i.e., Node 1 5 55 100 etc.). To select all elements use the syntax “Node 1:#.” Elemental based results are extrapolated to the nodes and averaged.
Individual elements may be selected on which to display the marker plot. You may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.). To select all elements use the syntax “Elem 1:#.” Results are plotted at the element centroid and summed and averaged if necessary (for nodal results).
Marker plots can be limited to only selected groups. A selected group or groups must have elements or nodes in them otherwise the plot will not appear. A listbox allows selection of the group(s) to which the marker plot will be applied. This is handy in that the same finite element entities can belong to multiple groups. Only those groups selected will be displayed with a marker plot while all other non-selected groups will remain unaffected and retain their own display attributes.
Marker plots can be targeted at only those finite elements which have certain material properties assigned to them. A listbox appears allowing selection of the materials for whose elements will be targeted for a marker display.
Properties
Marker plots can be targeted at only those finite elements which have certain element properties assigned to them. A listbox appears allowing selection of the properties for whose elements will be targeted for a marker display.
Element Types
Marker plots can be limited to only certain element types also.
5
5
106
PART 6
Results Postprocessing
In addition to targeting the entities, the marker plot can also be isolated to attributes of the entities as described in the following table. When nodes and elements are specifically targeted for the plot these choices are not available. However for any other target entities (groups, materials, properties, current viewport, element types), these choices are available:
Attribute
Nodes
Free Faces
Free Edges
Elements
Corners
Target
Deformations
Description
By default all marker plots are posted on the nodes of the target entities, including elemental based data. Elemental based data are extrapolated to the nodes, summed and averaged.
Marker plots can be posted on to all free faces of the target entities. The markers are posted at nodes on the free faces only. Elemental based data are extrapolated and averaged.
This will display a maker plot on the edges that only have one common element. The markers are posted at nodes on the free edges only.
Elemental based data are extrapolated and averaged.
Marker plots may be posted at element centroids. Data are summed and averaged for each element if necessary to produce a single data set for each element.
This will display markers only at corners of the model on nodes only.
Elemental based data are extrapolated and averaged.
By default, marker plots that are to be displayed on the deformed shape will be displayed on all deformation plots posted. You can select which deformation plots to target the marker plot to by selecting deformation plots form this listbox. This listbox will only appear when more than one deformation plot exists and is posted.
Important:
Once a target entity has been selected, it will remain the target entity for the marker plot until the user physically changes it.
CHAPTER 6
Marker Plots
107
6.3
Display Attributes
Marker plots can be displayed in various forms. Display attributes for marker plots are accessible by pressing the Display Attributes selection button on the Results application form with the Object set to Marker and the appropriate Method set (Scalar, Vector, or Tensor).
Toggles the form to change display attributes for marker plots with the method set to the type of desired marker (scalar, vector, or tensor).
describes in detail the marker plot attributes which can be modified. They differ for
each type of marker.
Attribute
Spectrum /
Constant
Show
Spectrum
Spectrum
Range
Title Editor
Show Title
Lock Title
Table 6-1 Common Marker Display Attributes
Description
This controls whether the marker colors (the vector arrows or other markers) are color coded according to the spectrum bar and value ranges or whether they are simply assigned different constant colors. If Constant is chosen you can select the colors for the resultant or components for vectors and tensors.
This toggle will remove or display the spectrum bar on the right of the current viewport. If the spectrum does not disappear from the graphics screen when the toggle is OFF, make sure other plots also do not have the spectrum turned ON.
This button will bring up the Spectrums form from which you can set the spectrum for the current viewport or create new spectrums. This form operates independently of the Results application. Therefore you do not need to press the Apply button in the Results application to effect changes in the spectrum. To learn more about changing the spectrum see
Display>Spectrums
(p. 306) in the MSC.Patran Reference Manual, Part 1:
Basic Functions.
This button will bring up a subordinate form for reassigning the range to the current spectrum in the current viewport. See
Display>Ranges
(p. 307) in the MSC.Patran Reference Manual, Part 1: Basic Functions for details. Also from this form you can invoke the Ranges form for creating and modifying new ranges. To learn more about changing ranges see
Display>Ranges
(p. 307) in the MSC.Patran Reference Manual, Part 1: Basic
Functions.
Selecting this button opens a form that allows the marker plot title to be edited. See
If this toggle is ON, then a title for the marker plot is displayed. Otherwise no title is displayed.
If this toggle is ON, then the title for the marker plot is not modified by results form selections. Otherwise some results form selections modify the title.
5
5
108
PART 6
Results Postprocessing
Table 6-1 Common Marker Display Attributes (continued)
Attribute
Show Max/Min
Label Display
Show
Scalar/Vector/
Tensor Label
Label Style
Description
If this toggle is ON, then the maximum and minimum values of the selected results set are displayed in the viewport. Otherwise they are not displayed.
If this toggle is ON, then the marker label (value) will be displayed at each marker.
Show on
Deformed
You can change the style of the numbers displayed on the marker label from the subordinate form that appears when you press this button. Styles can be integer, fixed, or exponential with specification of the number of significant digits. Also the label color is controlled from this form.
The marker plot will be displayed on the deformed shape of the model if a deformation plot has also been posted to the current viewport. The marker plot will display on all deformation plots if more than one is posted to the viewport. If this is not desired, see
Attribute
Constant -
Colors
Scalar Scale
Scale Factor
Scale Style
Table 6-2 Scalar Display Attributes
Description
If Constant is selected as the display attribute for the scalars, all markers will be drawn with the same color.
The size of the marker can be constant or relative. Screen Constant scale will keep all markers the same size based on a percentage of the screen size set by the Scale Factor. This means markers will stay the same size no matter whether you zoom in on the model or not. Model Constant scale will keep all markers the same size based on a percentage of the model size set by the Scale Factor. Zooming in on the model will make the markers appear larger. Screen Scaled and Model Scaled will give variable size markers based on the value of the scalar result and scale each relative to the screen size or the model size set by the Scale Factor.
This scale factor scales the size of the marker as described above.
Scale marker styles are: (1) triangle, (2) filled triangle, (3) square, (4) filled square, (5) diamond, (6) filled diamond, (7) hourglass, (8) filled hourglass,
(9) cross, (10) filled cross, (11) circle, (12) filled circle, (13) dot, (14) sphere,
(15) shaded sphere, (16) brick, (17) shaded brick
CHAPTER 6
Marker Plots
109
Table 6-3 Vector Display Attributes
Attribute Description
Constant -
Colors
If Constant is selected as the display attribute for the vectors you will be presented with color selection icons for the different components or for a single resultant. This is dependent on whether you have chosen to display the individual components or only the resultant from the main Select
Results form. Component selection is represented as XX, YY, and ZZ for the three component directions of any coordinate system. These translate into
, ,
z
and
r
φ θ
for cylindrical and spherical coordinate systems respectively.
Vector Length
The length of the vector can be constant or relative. Screen Constant vector length will keep all vector lengths the same size based on a percentage of the screen size set by the Scale Factor. This means vectors will stay the same length no matter whether you zoom in on the model or not. Model
Constant vector length will keep all vector length the same size based on a percentage of the model size set by the Scale Factor. Zooming in on the model will make the vectors appear larger. Screen Scaled and Model
Scaled will give variable length vectors based on the magnitude of each component (the actual result associated with each vector) and scale each relative to the screen size or the model size set by the Scale Factor.
Scale Factor
Anchor Style
This scale factor scales the size of the actual vector length as described above.
The vectors can be anchored either at the tip of the head or at the base of the arrow.
Head Style
Line Style
One, two or no head can be placed on the end of a vector.
Line styles can be either a line or a cylinder.
5
5
110
PART 6
Results Postprocessing
Table 6-4 Tensor Display Attributes
Attribute Description
Constant - Colors
If Constant is selected as the display attribute for the tensor vectors you will be presented with color selection icons for the different components or for the principals. This is dependent on whether you have chosen to display the individual components or only the principals from the main Select Results form. Component selection is represented as XX, YY, ZZ, XY, YZ, and ZX for the six component directions of any coordinate system. These translate into
r
, ,
, ,
z
and
for cylindrical and spherical coordinate systems respectively.
For 2D components, only XX, YY, and XY are presented and for 2D principals on the maximum and minimum principals are presented.
For 3D display all components or principals are presented.
Vector Length
Scale Factor
(p. 108) description of vector length.
(p. 108) description of scale factor.
Head Style
Line Style
Show Tensor Box
- Color
Box Style
Box Scale
(p. 108) description of head style.
(p. 108) description of line style.
This toggle allows for the display of the tensor box around which are shown the components of the tensor. The color of this box is controllable.
The box can appear as either wireframe (see through) or filled
(opaque).
The same description for the length of the vectors applies for the size of
the box as displayed on the model. See
(p. 108) description of Vector Length.
Box Scale Factor
This scale factor controls the size of the tensor box.
Important:
Vectors and tensors will only animate properly if you set the Vector Length to
Scaled. Constant vector lengths will not animate. Only the labels and sign changes will change during an animation. Also, once a target entity has been selected, it will remain the target entity for the particular marker plot until the user physically changes it.
CHAPTER 6
Marker Plots
111
6.4
Plot Options
Marker plots have various options. Plot options for marker plots are accessible by pressing the
Plot Options selection button.
Toggles the form to select plot options for marker plots.
The following table describes in detail the marker tool options which can be modified:
Option
Coordinate
Transformation
Scale Factor
Filter Values
Averaging Domain
Description
Vector and tensor results to display marker plots can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the
MSC.Patran global system, a material coordinate system, element
IJK coordinate system or the nodal (analysis) coordinate system
depending on the type of result (vector, or tensor). See
(p. 305) for a definition of each coordinate system. The
default is no transformation, which will plot data in the coordinate frame as stored in the database. Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user. These can vary from node to node. Element data can be stored from the analysis code in any coordinate system. Note also that the analysis translators that import the results data into the database can transform results. Check with the appropriate translator guide.
This scale factor has the effect of simply scaling the results up or down by the specified amount. This will have an effect on the fringe plot but will not effect the spectrum range values.
By specifying a filter value, a gate will be used to keep values below a maximum, above a minimum, between a certain range, or at the exclusion of certain values. The default is none. If filtering is used, only elements which pass the filter gate will display a marker plot on them.
For element based result quantities that must be displayed at nodes, an averaging domain must be used since more than one result will exist for each node. There is a contribution from each element attached to any particular node. By default all entities which contribute are used. Alternatively you can tell the Results application to only average results from those elements that share the same material or element property, are from the same target entities, or have the same element type. For more detail see
5
5
112
PART 6
Results Postprocessing
Option Description
Averaging Method
Extrapolation
Method
Complex No. as
The method in which certain results are determined can make a difference to the actual displayed plot. This is important when derived results from element based tensor or vector results are used such as von Mises stress or Magnitude displacements. For instance if you average at the nodes first and then derive the desired quantity you may get a different answer than if you derive first and then average. It is left up to the user to decide which is correct. For more detail see
Many times element based results that are to be displayed at nodes exist at locations other than the nodes such as at integration points.
Various methods are available to the user to extrapolate these results out to the nodes. For more detail see
The Real component of a complex number is the default by which results will be postprocessed. To force the postprocessor to use a different quantity such as Magnitude, Imaginary, Phase, or Angle, set this option pull down menu. This option will only be available if a complex result has been selected. It is not recommended to calculate invariants (e.g., von Mises) from complex results because the phase is not accounted for.
Existing
Scalar/Vector/
Tensor Plots
Save
Scalar/Vector/Tensor
Plot As
This listbox displays all existing marker plots. You may select one of these plots from the listbox and all settings of that plot including display attributes, target entities, option, and selected results will be restored. This is an easy mechanism to help make many plots with the settings of an existing plot without modifying the selected plot.
When the Action is set to Modify, this listbox appears under the
Select Results display of the Results application form.
Marker plots can be saved by name and recalled later for graphical display. Multiple marker plots can be saved in the database and displayed simultaneously. Be aware that when multiple marker plots are displayed simultaneously there could be some display problems if they are displayed on the same entities. These marker plots can be posted/unposted and deleted as explained in
Post/Unpost
(p. 25) and
Delete
(p. 27) respectively. Once a plot has been created and named it retains all results, attributes, target entities, and options assigned to it. If no plot name is specified a default is created called default_Scalar, default_Vector
or default_Tensor
. As long as no plot name is specified, the default name will be overwritten each time a plot is created or modified.
Important:
Once plot options have been selected, they will remain in effect for the marker plot until the user physically changes them.
CHAPTER 6
Marker Plots
113
6.5
Examples of Usage
The following are some typical scenarios for usage of the Marker plot tool. These instructions assume that the Action is set to Create and the Object is set to Marker unless otherwise specified.
Create a Scalar Plot
1. Set the Method to Scalar.
Method:
Scalar
2. From the Select Results form (left most icon) select the
Result Case from the first listbox. If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle
OFF and then select the Result Case.
3. Select the Scalar Result from the next listbox.
4. (Optional) If the result selected in the above listbox is a vector or tensor then select the scalar quantity to be derived from the selected vector or tensor result by selecting an item from the Quantity pull-down.
Quantity:
5. Press the Apply button with the Animate toggle OFF.
von Mises
Apply
5
5
114
PART 6
Results Postprocessing
Create a Vector Plot of Displacement Data
1. Set the Method to Vector.
Method:
Vector
2. From the Select Results form (left most icon) select the
Result Case from the first listbox. If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle
OFF and then select the Result Case.
3. Select the Vector Result (displacement) from the next listbox.
4. (Optional) Decide whether you want to display the vector plot as a resultant (single value) or as components (three values) with the Show As pull-down.
Show As:
Resultant
5. (Optional) If components are selected, toggle ON or OFF the components that you wish to display.
6. Press the Apply button with the Animate toggle OFF.
XX YY
Apply
ZZ
It is generally best to turn the vector labels OFF when plotting on the entire model. The display can get very cluttered with labels. This is done by pressing the Display
Attributes icon and turning OFF the Show Vector Label toggle.
Show Vector Labe
Z
Y
X
Z
Y
X
Figure 6-1 Resultant and Component Vector Plots of Displacement on Cantilever Plate
(constant vector lengths).
CHAPTER 6
Marker Plots
115
Create a Tensor Plot of Principal Stresses
1. Set the Method to Tensor.
Method:
Tensor
2. From the Select Results form (left most icon) select the
Result Case from the first listbox.
3. Select the Tensor Result (component stresses) from the next listbox.
4. (Optional) If more than one layer exists for these results, select the layer using the result Position button.
5. Decide which principals you want to display in the tensor plot with the Show As pull-down, and turning ON or OFF the desired components.
6. Press the Apply button with the Animate toggle OFF.
Position...(at Z1)
Show As: Principal
Max Mid Min
Apply
It is generally best to turn the Tensor Labels OFF when doing this on the entire mode to reduce label display clutter. This is done by pressing the Display Attributes icon and turning OFF the Show Tensor Label toggle.
Show Tensor Labe
5
Z
Y
X
Figure 6-2 Principal Tensor Plot of Stresses on Cantilever Plate
(constant vector lengths).
5
116
PART 6
Results Postprocessing
Animate a Static Scalar, Vector or Tensor Plot
1. Follow the general instructions to
Create a Vector Plot of Displacement Data
Create a Tensor Plot of Principal Stresses
(p. 115) for a vector or tensor plot respectively regardless
of the actual result to be plotted, but do not press the
Apply button.
2. Turn the Animate toggle ON on the main mode of the form.
3. (Optional) Press the Animation Options button icon.
Animate
4. (Optional) A modal style animation will result by default.
If a ramped style is preferred then change the Animation
By pulldown to Ramp.
5. Press the Apply button.
Animate by:Ramp
Apply
Animation will proceed and will oscillate from the minimum (zero) to the maximum display which is based on the scale factor for either the constant or scaled vector lengths. Change the vector length settings in Display
Attributes. Constant will make the animation appear as if only the labels and/or colors are changing unless the vectors change sign. Scaled will make the vectors appear to animate by scaling the actual size of the arrow based on result values.
Length: Model Scaled
CHAPTER 6
Marker Plots
117
Put a Scalar, Vector or Tensor on a Deformed Plot
1. Create a deformation plot and make sure it is posted to the current viewport. See
an explanation of deformation plot creation.
2. Now make a scalar, vector or tensor plot as explained in any of the examples above but don’t press the Apply button.
3. Press the Display Attributes icon button.
4. Turn ON the Show on Deformed toggle.
5. Press the Apply button with the Animate toggle OFF.
Show on Deform
Apply
5
Z
Y
X
Figure 6-3 Vector Plot on a Deformed Shape (scaled vector lengths).
Display a Transient Scalar, Vector or Tensor Animation
1. Set the Method to Scalar, Vector or Tensor as desired.
Method:
Tensor
2. From the Select Results form (left most icon) select the
Result Cases (time steps), from the first listbox, that you wish to include in the transient animation. You must select more than one. Use the mouse and the control key to select discontinuous selections or the shift key to select continuous selections. You can also use the Select button, when the
Result Cases are being displayed in abbreviated form, to filter and select the subcases (time steps) you want. In abbreviated form the Result Case name will only appear in the listbox as the name with number of subcases (time steps) selected, (i.e., Load Case 1, 6 of 41 subcases).
3. Select the Marker result from the next listbox.
4. (Optional) If the result quantity has more than one layer associated with it, select the layer from the result Position pull-down menu.
Position...(at Z1)
5
118
PART 6
Results Postprocessing
5. (Optional) If the results quantity is a tensor result and the
Method is set to Vector, select a resolved vector quantity from the result Quantity pull-down menu (such as
Maximum Principal stress).
Quantity:Max Principal
6. Turn the Animate toggle ON. (If the Animate toggle is OFF then the resulting plot will simply be a maximum plot of all selected Result Cases and will not animate.)
Animate
7. (Optional) Set the Vector Length to Model Scaled or Screen
Scaled under Display Attributes. This will result in the vector lengths being animated. Constant vector lengths will not animate and only the vector labels will change during
Length: Model Scaled
the animation.
8. Press the Animation Options icon button.
9. Select a global variable (time). Make any other optional modifications you want.
10. Press the Apply button. This method also works with load steps, frequency steps, or simply with multiple load cases that you may wish to animate.
Apply
Save a Scalar, Vector or Tensor Plot
1. Set up the marker plot as explained in previous examples, but do not press the Apply button.
2. Before pressing the Apply button to create a plot or animation, press the Plot Options icon button.
3. Type a name in the Save Scalar/Vector/Tensor Plot As databox.
Save Vector Plot As: myVector
4. Then press the Apply button.
Apply
Display Multiple Marker Plots
1. Set up the first marker plot as explained in previous examples, but do not press the
Apply button.
2. Save the marker plot as explained in
Save a Scalar, Vector or Tensor Plot
3. (Optional) Make a different viewport the active current viewport if desired. This is done by placing the cursor at the edge of the viewport and clicking with the mouse.
The current viewport will have a red border around it. This is the area where you click the mouse.
CHAPTER 6
Marker Plots
119
4. Repeat this process for as many marker plots as necessary and change the current viewport each time if desired.
Z
Y
X
Figure 6-4 Display of a Vector and a Tensor Plot in the Same Viewport.
Modify a Marker Plot or Animation
1. Set the Action to Modify with the Object set to Marker.
2. Set the Method to Scalar, Vector or Tensor as desired.
5. Press the Apply button at any time to see the results of your modifications.
Method:
Tensor
3. Select an existing marker plot from the Existing
Scalar/Vector/Tensor Plots listbox.
4. Change results, target entities, display attributes, plot or animation options as required.
Existing Vector Plots...
Apply
5
Z
Y
X
Figure 6-5 A Tensor Plot on the Cantilever Beam
Modified to Display in Crow’s Feet Form.
5
120
PART 6
Results Postprocessing
Display Multiple Animations in the Current Viewport
1. First create and save the marker plots (transient or static) as explained in
not animate them. Do not turn ON the Animate toggle.
2. (Optional) Set the Action to Post and the Object to Plots.
Post the plots to the viewports that you want if they are not already posted. They can be any plot type that supports animation.
3. Set the Action to Create and the Object to Animation. One by one, select the posted plots that you wish to animate from
Animate by:Ramp
the top listbox and modify their animation method if
Update Tool
necessary. This is done by pressing the Update Tool button.
4. Press the Apply button. See
details on this method.
Apply
MSC.Patran Reference Manual, Part 6: Results PostprocessingC
CHAPTER
7
Cursor Plots
■
■
■
■
■
6
122
PART 6
Results Postprocessing
7.1
Overview
For an overview of how the Results Application works please see
(p. 1). Cursor plots interactively display labels of either scalar, vector or tensor results
on the model. To specifically make or modify a cursor plot select Create or Modify from the Action pulldown menu on the Results Display form; and select Cursor from the Object pull-down menu. Then set the
Cursor type to Scalar, Vector or Tensor from the Method pull-down menu.
Application Form
Method
Attributes and
Options Toggles
•
Select Results
Scalar cursor plots display labels representing the scalar result value at the selected entities. Vector cursor plots display three labels, one for each of the vector components, in a column vector format. Tensor cursor plots display six labels in the lower triangular portion of a 3x3 matrix.
Typically results for tensor cursor plots are stress components.
This default setting establishes the application form to select the results used for the cursor plot.
•
Display Attributes Changes the application form to shows display attributes available.
•
Plot Options
Changes the application form to show the plot options available.
Select Result Case(s)
Specifies a results case to use for the cursor plot.
Select Cursor Result
Sets the result from the available scalar, vector, or tensor results list.
CHAPTER 7
Cursor Plots
123
6
6
124
PART 6
Results Postprocessing
Creating and Modifying a Cursor Plot
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a new Cursor plot and Modify is used to change an existing one. If you try to modify an existing plot with Create you will be asked for overwrite permission whereas
Modify assumes that the action is desired, so no overwrite permission is requested.
To create a Cursor plot the following basic steps must be followed:
1. Set the Action to Create or Modify, the Object to Cursor and the Method to Scalar,
Vector or Tensor.
2. Select a Result Case or Cases from the Select Results Case(s) listbox.
3. Select a result from the Select Scalar, Vector or Tensor Result listbox.
4. If more than one layer is associated with the results, select the layer (using the Position button) you wish to plot. These can be top or bottom results of shell elements, beam locations or laminate layers.
5. Optionally change the result Quantity. This is only possible if the selected result allows for this. If a tensor result has been selected for a vector Cursor plot, it must be resolved to a vector value. If a tensor or vector result has been selected for a scalar Cursor plot, it must be resolved to a scalar value. The various resolutions are:
Tensor to Vector:
Vector to Scalar:
Tensor to Scalar:
Minimum Principal, Middle (intermediate) Principal, Maximum
Principal, Component, Minimum Principal 2D, Maximum
Principal 2D
Magnitude, X component, Y comp., Z comp.
von Mises, XX, YY, ZZ, XY, YZ, XZ, Maximum Principal,
Middle Principal, Minimum Principal, Hydrostatic, 1st Invariant,
2nd Invariant, 3rd Invariant, Tresca, Max Shear, Octahedral. See hypertextparatextDefault Fontp.\
Vector to Scalar:
Tensor to Scalar:
Magnitude, X Component, Y Component, Z Component von Mises, XX, YY, ZZ, XY, YZ, ZX, Maximum Principal,
Middle Principal, Minimum Principal, Hydrostatic, 1st Invariant,
2nd Invariant, 3rd Invariant, Tresca, Max Shear, Octahedral. See hypertextparatextDefault ¶ Fontp.\ ).
6. Optionally, change the target entity type. This is done in the Target Entity pull-down menu at the bottom of the main Select Results form.
CHAPTER 7
Cursor Plots
125
7. Optionally change display attributes, or invoke other plot options by changing these settings using the two other icons at the top of the form. These are described in detail later in this chapter.
8. Press the Apply button when ready to create the Cursor plot.
9. The Apply button causes the Cursor Data form to be created and displayed. The user may now select entities at which results values are desired. The result values are recorded in the spreadsheet on the Cursor Data form.
To modify an existing Cursor plot, simply follow the above procedure with the Action set to
Modify. However, you must first select an existing plot using the Existing Cursor Plots button on the main form where results are selected. When an existing Cursor plot is selected, all results, attributes, and options in the various widgets associated with that plot are updated to reflect that plot’s settings. You may then proceed to modify the plot.
By default a Cursor plot with the name default_Cursor will be created unless the user specifically gives a different name. Multiple
Cursor plots can be created by giving cursor plots unique names. Only one Cursor plot can be posted to the viewport. Each viewport can have its own Cursor plot or other plot types posted.
Each plot can have its own attributes. Each plot can also target or be displayed on separate entities and have its own associated options. These are detailed in the next sections.
Component selection is represented as XX, YY, and ZZ for the three component directions of any coordinate system. These translate into r, ?, z and r, ?, ? for cylindrical and spherical coordinate systems respectively.
6
6
126
PART 6
Results Postprocessing
Cursor Data Form
To display this form go to the Results Application
1. Set AOM menus to Create/Cursor/Scalar
2. Select a Result Case, select a cursor result and hit the apply button. (Note: There must be a results model and results in the database.
The cursor plot differs from the other graphical results plots, in that there is not an immediate graphical feedback when the Apply button is pushed on the main form The Cursor Data form is displayed instead. The user may then graphically select desired entities at which to display the result value labels. This form must be displayed for the cursor tool in order to the allow the selection of the targeted entities type. Once this form is exited the cursor tool will no longer be active. If the user wishes to use select more entities for an existing tool then the user must post the tool which will re-display this form.
The Summary textbox displays the title information for the Cursor Plot including cursor name, selected result cases, selected result type, target entity type and minimum and maximum values for selected result.
In this example the target entity type is set to nodes.
This select databox allows the user to interactively select nodes at which the result values will be displayed. The user may also manually type desired nodes into the select databox
The result values for the selected entities are displayed in this spreadsheet. The first column of data is always the Entity ID. Scalar, vector and tensor results have one, three and six column(s), respectively of additional data, A maximum of four visible columns are displayed in this spreadsheet.
Tensor results require the user to use the horizontal scroll bar to see the last three columns of data.
The data collected in the spreadsheet may be output to a file by pressing the Write Report Button. The
Report Setup button allows the user to customize the output of the report.
CHAPTER 7
Cursor Plots
127
Cursor Report Setup
The Cursor Report Setup form is used to change the default report setup for the Cursor plot. The cursor reports can be formatted in a variety of ways and with many options.
To display this form go to the Results Application
1. Set AOM menus to Create/Cursor/Scalar
2. Select a Result Case, select a cursor result and hit the apply button. (Note: There must be a results model and results in the database.)
3. Hit the Report Setup button on the Cursor Data form.
The cursor data may be output by either overwriting or appending data to a file.
A file name can be specified in the File Name databox. A file browser is also available if you press the File button to select an existing file. The default cursor report filename is cursor_patran.prt.
A subordinate form will appear to allow for report formatting.
This is explained below in
Cursor Report Format
.
A subordinate form will appear to allow for selection of sorting options. This is described below in
Sorting Options
(p. 87)
6
6
128
PART 6
Results Postprocessing
Cursor Report Format
The Cursor Report Format is used to set the specific format of the data output to file including title text and alignment, pagination, column labels and the output format of the data. The formatting options are described in Cursor Report Format Options table.
[To display this form go to the Results Application
1. Set AOM menus to Create/Cursor/Scalar
2. Select a Result Case, select a cursor result and hit the apply button. (Note: There must be a results model and results in the database.)
3. Press the Report Setup button on the Cursor Data form.
CHAPTER 7
Cursor Plots
129
Cursor Report Format.
Below are descriptions for all the fields and settings for formatting cursor reports.
Table 7-1 Cursor Report Format Options
Item
File Width
Lines/Page
Top Margin
Left Margin
Pagination
Page Number
Edit
Alignment
Title/Header/Footer
Text Format
Input Column/
Label/Format
Column
Description
Sets the number of characters that can fit in the width of a page including spaces. The default is 128 characters.
Sets the number of lines per page. The default is 52 lines per page.
Sets the number of lines used to form a top margin. The bottom margin is set by the number of Lines/Page.
Sets the number of characters used to make a left margin. The right margin is set by the File Width.
If you wish to use pagination turn this toggle ON. The Page Number setting will appear to set the beginning page number. No footer or header information will be printed.
Set the beginning page number with this option. This databox only appears if Pagination has been turned ON.
This is an option menu for editing the Title, Footer, or Header. No
Footer or Header is allowed if pagination is OFF. This text box below this menu will update to allow for editing of the selected text.
Alignment of the report can be from the left margin, right margin or the report can be centered.
This textbox allows for inclusion and modification of a Title, Header or Footer. Which is set for editing is determined by the Edit option menu above this text box. A %I% may be placed in any of these text boxes to include the page number if Pagination has been turned ON.
A %rN% may also be included for adding additional blank lines.
These formatting characters are explained below.
This is a databox that becomes active to allow for changes in the actual Column Labels or Value Formats. Simply click on a cell in the spreadsheet that appears below this databox and the databox will become active to allow you to change the cells contents.
This is the column number with its associated label and value format.
6
6
130
PART 6
Results Postprocessing
Column Label
Value Format
This is the label that appears above the column of results. By default it is the same as results quantities selected. To change a label, select the cell and then change the value in the databox above. Press the
Enter or Return key to effect the change.
Results formats are listed in this column. They specify how the actual results values will be formatted in the report. They consist of the format characters surrounded by percentage signs. To change one of these formats, click on the cell that contains the format to change and enter your changes in the databox above the spreadsheet. Press the Enter of Return key to effect the change. The different characters and combinations acceptable for these formats is explained in .
Format Strings.
The format string is a description of how to convert integer, real, and string data to a formatted output. It is necessary to use a format string in the Value Format column in the spreadsheet to specify how to format the results values in the report. Some of these formats can also be used in the Title, Header and Footer. The format string is a simple character string which contains both raw text to output, and format specifiers, enclosed by a set of percent characters, which control how data items are formatted and output. Upper case letters (I, F, E, etc.) are interpreted literally and lower case letters are to be substituted with the appropriate values.
To change a value format simply click the mouse button with the cursor in the cell whose format you wish to change. Then in the Input databox above the spreadsheet change the value format to what you want and then press the Return or Enter key.
Table 7-2 Value Format Strings for Formatting Text Report Numbers
%%
Format
%Im%
%Fm.n%
Description
The simplest form of format specifier is a double percent to produce a single percent in the final output. Used if you want a percent character in the Title, Header or Footer.
Integer (I) specifier. This format specifier takes an integer value such as a node or element (entity) ID or other integer result for formatting. The value of “m” is the minimum number of characters to produce from the format. If “m” is omitted, then the exact number of characters necessary to hold the integer is used. The exact format produced is an optional minus sign followed by one or more digits. The default for integer data is %I6%.
Fixed (F) float specifier. This format specifier takes a real results value for formatting in fixed point notation. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters necessary to hold the conversion is used.
The value of n is the number of decimal digits to produce. If omitted, then all significant digits will be produced. The exact format produced is an optional minus sign followed by zero or more digits, a decimal point, and zero or more digits. At least one digit will precede or follow the decimal point. The default for real data is %F12.6%.
%Em.n.p%
%Gm.n.p%
%Sm%
%rN%
CHAPTER 7
Cursor Plots
131
Exponential (E) float specifier. This format specifier takes a real value for formatting in scientific exponential notation. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters necessary to hold the conversion is used. The value of n is the number of decimal digits to produce. If omitted, then all significant digits will be produced. The value of p is the number of digits to display before the decimal point, and defaults to one. If zero is specified, then a single zero precedes the decimal point. The exact format produced is an optional minus sign followed by zero or more digits, a decimal point, zero or more digits, a capital E, a plus or minus sign, and two decimal digits. At least one digit will precede or follow the decimal point. The default value for read data is the F format.
General (G) float specifier. This format specifier takes a real value for formatting in either F or E format. The format used depends on the value of the number to convert. In general, if the exponent is small, the F format will be used, otherwise the E format is used. See the descriptions of the F and E formats.
String (S) specifier. This format specifier takes the next string value from the character data array for formatting. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters in the string is used. The default value for string data is %S32%.
New (N) line specifier. This format specifier causes a new line to be started. The previous line is output as is, and formatting starts at column one of the new line. The value of r is a repeat count for skipping multiple lines. If output is to a string, then new line characters will be written to the string. This is used in the Title, Header and Footer text.
6
6
132
PART 6
Results Postprocessing
Variables.
Variables can be placed in titles, footers, or headers of reports. The variables available are shown in the table below. Be sure to place the $ symbol in front of the variable otherwise it will not be recognized as a variable.
Table 7-3 Value Format Strings for Formatting Text Report Numbers
Format
$LC_NAME
$SC_NAME
$PRES_NAME
$SRES_NAME
$LYR_NAME
$DATE
$PAGE
$NNODES
$MAXNOD
$DEFMAX
$NDMAX
$NWIDTH
$DATA_TITLE
$PRODUCT
$DB_NAME
$JOB_NAME
$CODE_NAME
Description
This is the Result Case (load case) name.
This is the subcase name.
This is the primary result name.
This is the secondary result name.
This is the result layer name.
The current date and time in the format dd-mmm-yy hh:mm:ss.
The current report page number.
The number of nodes in the report. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case. Typically used to create MSC.Patran nodal (nod) result files.
The highest ID of a node in the file. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case. Typically used to create MSC.Patran nodal (nod) result files.
The maximum value encountered within the file. Variable is printed in
E15.6 format if left aligned. Valid for nodal report only, sorted by Result
Case. Typically used to create MSC.Patran nodal (nod) result files.
The ID of the node with the maximum value. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case.
Typically used to create MSC.Patran nodal (nod) result files.
The number of columns in the file. This will be the number of results quantities output to the report. Note that the Entity Id which is the first column of most reports by default is not included in NWIDTH. It is actually the number of columns of real, floating point data. Typically this is used to create MSC.Patran nodal (nod) and elemental (els) result files.
The register title. You must use the built in function res_data_title() to set a title for your register. Once this title is set, then it will show up when you use $DATA_TITLE.
The MSC.Patran product/version.
The name of the current database.
The name of the analysis job.
The name of the analysis code as set under Preferences/Analysis.
CHAPTER 7
Cursor Plots
133
$GV:<name>
$LEFT
$MIDDLE
$RIGHT
The name and value of an associated global variable such as time, frequency, eigenvector, etc. If a global variable is one word then all that is needed is to specify that global variable after the colon, i.e.,
$GV:Time. However, if a global variable name has a space in it or, that is, consists of more than one word, you must surround the name with single quotes, i.e., $GV:’Design Cycle.’ Failing to do this will results in the variable picking up only the first word and will not find the correct global variable and will report garbage. Using this variable in the header and footer when multiple results cases (multiple GVs) will only use the first global variable encountered.
Aligns the current line of text to the left, overriding the global page alignment.
Aligns the current line of text to the middle, overriding the global page alignment.
Aligns the current line of text to the right, overriding the global page alignment.
6
6
134
PART 6
Results Postprocessing
Sorting Options
Results can be sorted in a report and sorting is controlled via this form which is available from the Cursor Report Setup form by pressing the Sort button.
Sorting Options
Sort Order
Ascending
Sort By
Algebraic Value
Absolute Value
Sort Data By
Entity ID
Magnitude
Descending
Results can be sorted in Ascending (from smallest to largest) or Descending order. Ascending order is the default.
Sorting can be done by comparing Algebraic Values which considers the sign of a value. A negative value will be treated as less than a positive number. Or the Absolute Value of the results can be used where sign is ignored, and the relative size in magnitude is considered in the sort.
This listbox displays the result entity by which the sort is based. By default sorting is always done and is based on the
Entity ID. This would be a node or element number in general.
OK
CHAPTER 7
Cursor Plots
135
7.2
Target Entities
Cursor plots can be displayed on various model entities. By default Cursor plots are targeted on all nodes displayed in the current viewport regardless of the results data type (elemental or nodal based). To change target entity selection for Cursor plots, select an entity type from the
Target Entity option menu on the Select Results form.
The following table describes in detail which entities Cursor plots can be targeted.
Entity
Nodes
Elements
Description
Individual nodes may be selected on which to display the Cursor plot.
You may type in any node numbers manually or by selecting them graphically from the screen. Be sure to include the word Node in front of the IDs you type in manually, (i.e., Node 1 5 55 100 etc.). Elemental based results are extrapolated to the nodes and averaged.
Individual elements may be selected on which to display the Cursor plot. You may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.).Results are plotted at the element centroid and summed and averaged if necessary (for nodal results).
Isosurfaces
Streamline
Path
6
Important:
Once a target entity type has been selected, it will remain the target entity type for the
Cursor plot until the user physically changes it.
6
136
PART 6
Results Postprocessing
7.3
Display Attributes
Cursor plots can be displayed in various forms. Display attributes for Cursor plots are accessible by pressing the Display Attributes selection button on the Results application form with the
Object set to Cursor and the appropriate Method set (Scalar, Vector or Tensor).
Toggles the form to change display attributes for Cursor plots with the method set to the type of desired Cursor (scalar, vector or tensor).
Attribute
Title Editor
Show Title
Lock Title
Label Style
Show on Deformed
Table 7-4
Common Cursor Display Attributes
Description
Selecting this button opens a form that allows the cursor plot title to be edited. See
If this toggle is ON, then a title for the cursor plot is displayed.
Otherwise no title is displayed.
If this toggle is ON, then the title for the cursor plot is not modified by results form selections. Otherwise some results form selections modify the title.
You can change the style of the numbers displayed on the
Cursor label from the subordinate form that appears when you press this button. Styles can be integer, fixed, or exponential with specification of the number of significant digits. Also the label color is controlled from this form.
The Cursor plot will be displayed on the deformed shape of the model if a deformation plot has also been posted to the current viewport. The
CHAPTER 7
Cursor Plots
137
7.4
Plot Options
Cursor plots have various options. Plot options for Cursor plots are accessible by pressing the
Plot Options selection button.
Toggles the form to select plot options for Cursor plots.
The following table describes in detail the Cursor tool options which can be modified:
Option
Coordinate
Transformation
Scale Factor
Averaging Domain
Averaging Method
Extrapolation
Method
Description
Vector and tensor results to display Cursor plots can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the MSC.Patran global system, a material coordinate system, element IJK coordinate system or the nodal (analysis) coordinate system depending on the type of result (vector, or tensor). The default is no transformation, which will plot data in the coordinate frame as stored in the database. Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user. These can vary from node to node. Element data can be stored from the analysis code in any coordinate system. Note also that the analysis translators that import the results data into the database can transform results. Check with the appropriate translator guide.
This scale factor has the effect of simply scaling the results up or down by the specified amount.
For element based result quantities that must be displayed at nodes, an averaging domain must be used since more than one result will exist for each node. There is a contribution from each element attached to any particular node. By default all entities which contribute are used. Alternatively you can tell the Results application to only average results from those elements that share the same material or element property, are from the same target entities, or have the same element type.
The method in which certain results are determined can make a difference to the actual displayed result value. This is important when derived results from element based tensor or vector results are used such as von Mises stress or Magnitude displacements. For instance if you average at the nodes first and then derive the desired quantity you may get a different answer than if you derive first and then average. It is left up to the user to decide which is correct.
Many times element based results that are to be displayed at nodes exist at locations other than the nodes such as at integration points.
Various methods are available to the user to extrapolate these results out to the nodes.
6
6
138
PART 6
Results Postprocessing
Existing Cursor
Plots
This listbox displays all existing Cursor plots. You may select one of these plots from the listbox and all settings of that plot including display attributes, target entities, option, and selected results will be restored. This is an easy mechanism to help make many plots with the settings of an existing plot without modifying the selected plot.
When the Action is set to Modify, this listbox appears under the
Select Results display of the Results application form.
Save Cursor Plot As
Cursor plots can be saved by name and recalled later for graphical display. Multiple Cursor plots can be saved in the database. These
Cursor plots can be posted/unposted and deleted respectively.
Once a plot has been created and named it retains all results, attributes, target entities, and options assigned to it. If no plot name is specified a default is created called default_Cursor. As long as no plot name is specified, the default name will be overwritten each time a plot is created or modified.
Important:
Once plot options have been selected, they will remain in effect for the Cursor plot until the user physically changes them.
CHAPTER 7
Cursor Plots
139
7.5
Examples of Usage
The following are some typical scenarios for usage of the Cursor plot tool. These instructions assume that the Action is set to Create and the Object is set to Cursor unless otherwise specified.
Create a Cursor Plot of von Mises Stress
1. Set the Method to Scalar.
Method:
Scalar
2. From the Select Results form (left most icon) select the Result Case from the first listbox.
If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle
OFF and then select the Result Case.
6
3. Select the Stress Tensor from the Select Cursor Result listbox.
4. Select von Mises from the result Quantity menu.
Quantity: von Mises
5. Set the entity type from the Target Entity menu to Elements.
Target Entity:
Elements
6. Press the Apply button.
Apply
140
PART 6
Results Postprocessing
7. Once the Cursor Data Form is displayed the user may graphically select the desired entities. The von Mises value will be displayed on the model.
6
Figure 7-1 Cursor Plot of von Mises stress.
Create a Cursor Plot of Displacement Data
1. Set the Method to Vector.
Method:
Vector
2. From the Select Results form (left most icon) select the Result Case from the first listbox.
If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle
OFF and then select the Result Case.
3. Select the Displacements from the Cursor Result listbox.
4. Set the entity type from the Target Entity menu to Nodes.
Target Entity:
Nodes
CHAPTER 7
Cursor Plots
141
5. Press the Apply button.
Apply
6. Once the Cursor Data Form is displayed the user may graphically select the desired nodes. The displacement components will be displayed on the model.
Figure 7-2 Cursor Plot of Vector Components of Displacement.
Create a Tensor Plot of Stresses
1. Set the Method to Tensor.
Method:
Tensor
2. From the Select Results form (left most icon) select the Result Case from the first listbox.
3. Select the Stress Tensor from the Cursor Result listbox.
4. (Optional) If more than one layer exists for these results, select the layer using the result
Position button.
Position...(at Z1)
5. Set the entity type from the Target Entity menu to Elements.
Target Entity:
Elements
6
6
142
PART 6
Results Postprocessing
6. Press the Apply button.
Apply
7. Once the Cursor Data Form is displayed the user may graphically select the desired elements. The stress components will be displayed on the model.
Figure 7-3 Stress Components.
Put a Cursor on a Deformed P
lot:
1. Create a deformation plot and make sure it is posted to the current viewport. See for an explanation of deformation plot creation.
2. Now make a cursor plot as explained in any of the examples above but don’t press the
Apply button.
3. Press the Display Attributes icon button.
4. Turn ON the Show on Deformed toggle.
Show on Deformed
5. Press the Apply button.
Apply
CHAPTER 7
Cursor Plots
143
6
Figure 7-4 Cursor Plot on a Deformed Shape .
6
144
PART 6
Results Postprocessing
Save a Cursor Plot
1. Set up the Cursor plot as explained in previous examples, but do not press the Apply button.
2. Before pressing the Apply button to create a plot, press the Plot Options icon button.
3. Type a name in the Save Cursor Plot As databox.
Save Cursor Plot As: myvonMisesCursor
4. Then press the Apply button.
Apply
Report of Cursor Data
1. After creating a cursor plot and populating the Cursor Data form spreadsheet with the desired values, the data in spreadsheet may be output to a file.
2. By default, a new file will be created called patran_cursor.prt
3. If the user wishes to customize the report, formatting and sorting options are available from the Report Setup form. To access these, press the Report Setup button on the
Cursor Data form.
Report Setup...
4. Press the Write Report button to generate a report file.
Write Report
Write Report
The report should look somewhat similar to this:
Figure 7-5 Report of Displacement Data with Summary.
MSC.Patran Reference Manual, Part 6: Results PostprocessingC
CHAPTER
8
Graph (XY) Plots
■
■
■
■
■
7
134
PART 6
Results Postprocessing
8.1
Overview
For an overview of how the Results Application works please see
(p. 1). To specifically make or modify a graph plot select Create or Modify from the
Action pull-down menu on the Results Display form; and select Graph from the Object pull-down menu.
Presently only Y vs X plots may be created.
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a new graph plot and Modify is used to change an existing one. If you try to modify an existing plot with Create you will be asked for overwrite permission whereas Modify assumes that the action is desired, so no overwrite permission is requested.
Toggles the form to select results for graph plots. This is the default mode of the Graph form.
For both Modify and Create the same basic operations and options are available. To create or modify a graph plot the following basic steps must be followed:
1. Set the Action to Create or Modify and the Object to Graph.
2. Select a Result Case or Cases from the Select Results Case(s) listbox.
(p. 15) for a detailed explanation of this process
as well as
3. Set the Y-axis value to either a Results value or a Global Variable if multiple Result Cases are selected. The Global Variables available depend on the result type but are generally time, frequency or load step. If a Result value is chosen, then select the result from the Select Y
Result listbox otherwise select a Global Variable. Global variables will only be available if multiple Result Cases have been selected. Skip to step 5 if a global variable has been set for the Y-axis.
4. For Result Y-axis values, if more than one layer is associated with the result, select the layer (using the Position button) you wish to plot.
CHAPTER 8
Graph (XY) Plots
135
5. For Result Y-axis values, optionally change the results Quantity. This is only possible if the selected result allows for this. If a vector or tensor result has been selected for a graph plot, it must be resolved to a scalar value. The various resolutions are:
ector to Scalar:
Magnitude, X Component, Y Component, Z
Component.
ensor to Scalar:
von Mises, XX, YY, ZZ, XY, YZ, XZ, Minor,
Intermediate, Major, Hydrostatic, 1st Invariant,
2nd Invariant, 3rd, Invariant, Tresca, Max Shear,
Octahedral. See
6. Set the X-axis value to either to Result, Global Variable, Coordinate
Axis, Path Length or Beams and select the necessary items as was done for the Y-axis values. More detailed explanations of the X- and Y-axis types are given below. Path Lengths (points, curves and element edges) and Beams are selected as target entities.
7. Select the target entities. For most plot types this is an optional activity but for a Graph plot it is required unless the graph is a global variable
versus another global variable. To do this press the
(p. 137) button icon and select the nodes, elements, beams, curves, or
path for which you wish to create an Graph plot.
8. Optionally change any display attributes, or invoke other plot options by changing these settings using the other two icon buttons at the top of the form. These are described in detail later in this chapter. See
9. Press the Apply button when ready to create the graph.
Apply
To Modify an existing graph, follow the above procedure with the exception that you must first select an existing plot using the Existing Graph Plots button on the main form where results are selected. When an existing graph is selected, all results, attributes, and options in the various widgets associated with that plot are updated to reflect that plot’s settings. You may then proceed to modify the plot.
By default a graph plot named default_Graph
will be created unless the user specifically gives a different name. Multiple graph plots can only be created and posted by giving separate names. Multiple graph plots can be posted to the same XY window or to separate XY windows. Each XY window can have its own set of graphs posted.
Each plot can have its own attributes. Each plot can also target or be associated with separate entities and have its own associated options. These are detailed in the next sections.
The Results application, when producing a graph, actually is driving the XY Plot application by creating
XY windows and curves and setting display attributes. It is important to understand the interaction between the XY Plot application and the Results application. Many more display attributes and other options are available and modifiable from the XY Plot application than can be controlled from the
Results application. Although a Graph plot can be posted/unposted and modified from the Results application, more versatile controls are found under XY Plot.
Care should also be taken when naming Graph plots in the Results application since each graph can create a new XY window with its own name. If two Graph plots share the same XY window, things may happen that do not quite make sense until you understand the interaction between Results and XY Plot.
See
Overview of the XY Plot Application
(Ch. 1) in the MSC.Patran Reference Manual, Part 7: XY
Plotting.
7
7
136
PART 6
Results Postprocessing
X and Y Axis Values.
The following table explains the different X and Y axis values and what each can be plotted against.
X or Y Value Description
Result
Path Length /
Beam
A result value on the Y-axis can be plotted against another results value for the selected target entities or it may be plotted against a global variable such as time, frequency, or load step. A Y-axis result value may also be plotted against coordinate locations, or locations along a curve or beam.
To select a result you simply select the result from the listbox presented whether it be for the X or the Y axis. A subordinate form will appear for the X-axis result selection but functions identically to that for the Y-axis.
Since only scale values can be plotted, you must select resolved values if a tensor or a vector is chosen. If multiple layers are associated with a result you must also select the desired layer such as top or bottom stresses of a plate element.
Global Variable
A global variable is a single value associated with a particular Result Case such as the time of a time step, the frequency of a mode shape, or the load step number of a non-linear analysis. These values can be plotted against result values (Y-axis) to give you transient type graphs or they can be plotted against other global variables (X-axis).
Coordinate
Result values (Y-axis) can be plotted against coordinate locations (X-axis).
To choose the X-axis coordinate, use the Select Coordinate Axis databox to graphically select the coordinate frame and the desired direction (vector component-
, ,
;
R
, ,
Z
;
R
Φ θ
) or points that define a vector direction. This is useful for plots such as a stress gradient as a function of distance from a hole.
You can define a geometric curve from which a graph may be generated where the X-axis is defined as the distance along the curve. Use the Target
Entities option to specify which curve, points, or edges/beams will actually make up the path. See
CHAPTER 8
Graph (XY) Plots
137
8.2
Target Entities
Graphs can be displayed for various model entities. There is no practical default for graph plots and some sort of target entity must be selected, be they nodes, elements, or paths. To change target entity selection for graph plots, press the Target Entities icon with the Object set to Graph.
Toggles the form to select target display entities for graph plots.
The following table describes in detail to which entities graph plots can be targeted. The entity types and their entity attributes are of course dependent on the type of graph you want and what you have selected as the Y-axis or X-axis quantity. Some combinations may not make any sense. For instance a global variable plotted against another global variable does not need the specification of target entities.
However, results quantities versus anything will need target entities specified.
Entity
Nodes
Elements
Groups
Materials
Description
Individual nodes may be selected from which to create a graph. Nodes are selected graphically from the screen and fill the databox. However, you may type in any node numbers manually. Be sure to include the word
Node in front of the IDs you type in manually, (i.e., Node 1 5 55 100 etc.).
Elemental based results are extrapolated to the nodes and averaged.
Individual elements may be selected from which to create a graph.
Elements are selected graphically from the screen and fill the databox.
However, you may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.). With elemental data, values will be extrapolated or averaged to the element centroid for reporting purposes.
Graphs can be limited to entities (nodes or elements) within a selected group. A selected group or groups must have elements or nodes in them otherwise the plot will not appear. A listbox allows selection of the group(s). Since groups can contain either nodes or element it is therefore also necessary to identify the entity attributes (nodes, element centroids, etc.) as explained in the following table.
As with groups, elements with certain material properties can be selected.
As with elemental data, values will be extrapolated or averaged to the element centroid for reporting purposes.
7
7
138
PART 6
Results Postprocessing
Entity
Properties
Path
Description
As with groups, elements with certain element properties can be selected.
As with elemental data, values will be extrapolated or averaged to the element centroid for reporting purposes.
A path can be defined in a variety of ways. The graph will be created by extrapolating results from the elements that touch the path to points that lie on that path. The path can be defined as a collection of points
(geometric grids or nodes), curves, or edges of surfaces and elements. A select listbox will appear to allow you to type in individual beams/curves/etc. or select them graphically from the screen. When typing in individual beam element IDs make sure the word “Elem” is in front of all the IDs, (e.g., “Elem 1 3 5 10 20:40 100:150:10.”). When a path is selected as the target entity and that path is defined by curves or beams/element edges, you need to also specify in an accompanying databox, the number of result locations to extract data from for the resulting plot. This is referred to as Points Per Segment in the Target
Entities form.
In addition to targeting the above entities for a graph plot, the graph must be isolated to attributes of the entities as described in the following table. When nodes or elements are specifically targeted for the plot these choices are not available. However, for group or path target entities, the following choices are available.
Attribute Description
Nodes
Element Centroids
Specifies the use of the nodes of the target entities for extraction of the results value. Elemental based data are extrapolated to the nodes and averaged.
Specifies that results be extracted at the element centroids for the plot. Nodal based data are summed and averaged at the centroid.
Points Per Segment
This is the number of points to be created for a graph using a Path as its Target Entity. The number of points generated in between selected nodes or curve end points is the number specified less one.
A point will always be created at node points and end points of curves or element edges. The number of points can be one (1) to any positive number.
Points
When a path is the target entity, Points specifies that results be extracted at geometric points along that path. You can select these points graphically which can be made up of nodes, points, intersections, screen positions, etc. If the Number of Segments is one (1), a point on the graph will be created for each node. If two (2) is specified then an intermediate point will be created between each node. The number of points per segment less one will be created
(interpolated) between points if greater than one (1). The path through the points will be piece wise linear (PWL). See notes below.
CHAPTER 8
Graph (XY) Plots
139
Curves
Attribute
Edges/Beams
Description
When a path is the target entity, specifies that path by the selection of geometric curves. These curves can be lines or edges of surfaces and elements. The select mechanism gives you control for defining all of these choices. If the Number of Segments is one (1), a point on the graph will be created for each end point of selected curves. If two (2) is specified then an intermediate point will be created between each end point. The number of points per segment less one will be created (interpolated) between end points and evaluated at equal arc lengths along each curve if greater than one (1). See notes below.
When a path is the target entity, specifies that path as beams or element edges. The number of points per segment less one (1) will be generated along each element edge. Midside nodes are not used by necessity. The points are generated at equal parametric locations along the edge using the order/geometry of the element to determine the locations. See notes below.
Notes on Path Target Entities:
1. The Point and Curve types have a dependency on the current group. This is important if you are working in small sections of a large model. The current group will limit the scope of the search for potential elements to contain the XYZ points generated. Thus selecting points that are not in the current group will result in no plot.
2. The Edges/Beam type is the most efficient interpolator. Since the elements are specified in the input, interpolation of results is a direct operation without any global searching for point mapping of global to parametric space.
3. When plotting versus Path Length, distances are calculated as straight line distances between interpolated points. If curves or edges are contiguous, the matching end points appear only once. If disjointed paths are specified, the distance value is reset to zero and the plot will zig-zag back to zero for the start of each disjointed section.
Important:
Once a target entity has been selected, it will remain the target entity for any graph until the user physically changes it.
7
7
140
PART 6
Results Postprocessing
8.3
Display Attributes
Graph plots can be displayed in various forms. Display attributes for graphs are accessible by pressing the
Display Attributes icon on the Results application form with the Object set to Graph.
Toggles the form to change display attributes for graph plots.
This section describes the graph plot attributes which can be modified. Only a limited number of display attributes are actually available under the Results application for graph plots. Once a graph plot has been created, you may make attribute changes to the curves, axis and other entities in the XY Window with the
XY Plot application (see
Overview of the XY Plot Application
(Ch. 1) in the MSC.Patran Reference
Manual, Part 7: XY Plotting).
Attribute Description
Curve Fit
Curve Style
Show Symbol
Curve fit options are Linear, Scatter, Spline, and Least Squares.
Linear is the default and will connect adjacent points with a linear line between the two. Scatter does not put any line on the plot at all but leaves just the points. Spline will connect the points with a curved and continuous line. This results in a smooth line with no abrupt changes is direction. Least Squares will do a least squares fit through all points to create one linear best fit line.
Curves can be solid, dotted, dashed, or dot-dashed.
This toggle turns ON or OFF the display of symbols. The symbol used is the default symbol of the XY Plot application (a yellow round dot).
Show X/Y Axis Label
This toggle will display the X- or Y-axis label if ON.
X/Y Axis Label
X/Y Axis Scale
This databox allows for specification of the X- and Y- axis label.
The X- and Y-axis scales can be set to linear or log with this switch.
Label Style
This button brings up a subordinate form to change the label style of numerical text such as the numbers on the X- and Y-axes. The numerical format can be changed to integer, fixed, or exponential with specifications of color, size, and significant digits.
CHAPTER 8
Graph (XY) Plots
141
Attribute
XY Window Name
Append Curves in XY
WIndow
Description
A XY Window name must be supplied in order to create a graph.
This will be the name of the separate graphical viewport for the graph that will appear on creation. Care should be taken when creating multiple graphs not to become confused. Even though you
can save a graph plot with at specific name, (see
(p. 142)), multiple plots can reference the same XY window.
Multiple plots will therefore appear in the same XY window even though they are actually separate Graph plot tools. The default XY window name is
Results Graph
.
If this toggle is ON, then additional curves that may be created in the same XY Window and associated to the same Graph plot as opposed to being overwritten. For instance, you may put up a transient displacement plot of Node 101 and then decide it would be nice to overlay the same results from Node 345 in the same plot.
However, care should be taken in that multiple graph plots can reference the same XY window and multiple curves in the same XY window of different data and magnitude can significantly change the axis scales and make plots unreadable.
Important:
Once plot attributes have been selected, they will remain in effect for any graph plot until the user physically changes them.
7
7
142
PART 6
Results Postprocessing
8.4
Plot Options
Graph plots have various options. Plot options for graphs are accessible by pressing the Plot Options button icon on the Results Display form.
Toggles the form to select plot options for graph plots.
The following table describes the graph options which can be modified:
Option Description
Coordinate
Transformations
Scale Factor
Filter Values
Vector and tensor results for displaying graph plots can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the MSC.Patran global system, a material coordinate system, element IJK coordinate system or the nodal (analysis) coordinate system depending on the type of result
(vector, or tensor). See
each of these coordinate systems. The default is no transformation, which will extract data in the coordinate frame as stored in the database. Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user. These can vary from node to node. Element data can be stored from the analysis code in any coordinate system.
This scale factor has the effect of simply scaling the results up or down by the specified amount. For results data this will scale both the x and y axes.
By specifying a filter value, a gate will be used to keep values below a maximum, above a minimum, between a certain range, or at the exclusion of certain values. The default is none. If filtering is used, only those results which pass the filter gate will be used in the graph plot.
The filter values apply only to the Y-axis data.
Averaging
Domain
For element based result quantities that must be extracted at nodes, an averaging domain must be used since more than one result will exist for each node. There is a contribution from each element attached to any particular node. By default all entities which contribute are used.
Alternatively you can tell the Results application to only average results from those elements that share the same material or element property, are from the same target entities, or have the same element type. For more detail see
Averaging Method
The method in which certain results are determined can make a difference to the actual displayed plot. This is important when derived results from element based tensor or vector results are used such as
VonMises stress or Magnitude displacements. For instance if you average at the nodes first and then derive the desired quantity you may get a different answer than if you derive first and then average. It is left up to the user to decide which is correct. For more detail see
CHAPTER 8
Graph (XY) Plots
143
Option
Extrapolation
Method
Complex No. as
Existing Graph
Plots
Save Graph Plot
As
Description
Many times element based results that are to be extracted from the nodes exist at locations other than the nodes such as at integration points. Various methods are available to the user to extrapolate these
results out to the nodes. For mode detail see
The Real component of a complex number is the default by which results will be postprocessed. To force the postprocessor to use a different quantity such as Magnitude, Imaginary, Phase, or Angle, set this option pull down menu. This option will only be available if a complex result has been selected. It is not recommended to calculate invariants (e.g., von Mises) from complex results because the phase is not accounted for.
This listbox displays all existing graph plots. You may select one of these plots from the listbox and all settings of that plot including display attributes, target entities, option, and selected results will be restored. This is an easy mechanism to help make many plots with the settings of an existing plot without modifying the selected plot. When the Action is set to Modify, this listbox appears under the Select Results display of the Results application form also.
Graph plots can be saved by name and recalled later for graphical display. Multiple graph plots can be saved in the database and displayed simultaneously. These graph plots can be posted/unposted
respectively. Once a plot has been created and named it retains all results, attributes, target entities, and options assigned to it. If no plot name is specified a default is created called default_Graph
. As long as no plot name is specified, the default_Graph
will be overwritten each time a plot is created or modified.
7
Important:
Once plot options have been selected, they will remain in effect for any subsequent graph plot until the user physically changes them. Also for graph plots be aware that although the name is saved in the database and all attributes attached to it, the user can inadvertently delete or modify XY Windows, Curves, and other attributes associated with a graph plot in the XY Plot application. This is because each graph plot creates a XY Window and Curves which then become available in the XY Plot application. If you delete a XY Window in the XY Plot application you will affect any graph plot referencing that XY Window. See
7
144
PART 6
Results Postprocessing
8.5
Examples of Usage
The following are some typical scenarios for usage of the Graph plot tool. These instruction assume that the Action is set to Create and the Object is set to Graph unless otherwise specified.
Graph of Results Versus Coordinate Distance (Nodal)
Displacement results are used in this example.
1. From the Select Results form (left most icon) select the
Result Case from the first listbox. If more than one subcase exists for a Result Case, turn the Abbreviate Subcases toggle
OFF and then select the Result Case.
2. The Y-axis should be set to Result values.
3. Select the Y-axis result quantity (Displacements) from the
Select Y Result listbox.
Y:
Result
4. (Optional) Set the result Quantity to Magnitude for displacement results.
5. Set the X-axis to Coordinate and then either select the coordinate from the graphics screen or type in the coordinate value (Coord 0.1). Make sure you are selecting the correct coordinate axis. Use the select mechanism if necessary (Coord 0.1 indicates coordinate frame ID zero and the 1 or x direction.)
6. Use the Target Entities form to select the desired nodes. The nodes used in this example are indicated on the beam shown in
Quantity: Magnitude
X:
Coordinate
7. Press the Apply button.
Apply
X-Direction (Inches)
Figure 8-1 Result Value (Displacement) Versus
Distance of the Cantilever Beam’s Nodes as Shown.
CHAPTER 8
Graph (XY) Plots
145
Graph of Results Versus Results (Nodal)
Displacement versus stress results are used in this example.
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. The Y-axis should be set to Result values.
3. Select the Y-axis result quantity (displacement) from the
Select Y Result listbox.
4. (Optional) Set the result Quantity if necessary (to
Magnitude for this example).
5. (Optional) If more than one layer exists for these results, also select the layer you wish to plot.
6. Set the X-axis to Result.
Y: Result
Quantity: Magnitude sition...(NON-LAYERED
X:
Result
7. Similar to the Y-axis, you must select results for the X-axis.
Quantity: von Mises
This is done in a subordinate form similar to selecting results for the Y-axis. Repeat steps
Position...(at Z1)
axis.
8. Use the Target Entities form to select nodes as target entities. Graphically select the nodes from the screen after setting the target entities to nodes.
9. (Optional) Use the Display Attributes form to make any changes to the display attributes of the plot.
10. Press the Apply button.
The order in which the results will be plotted will be the sequence that the nodes were selected in Target Entities.
Apply
7 von Mises Stress (PSI)
Figure 8-2 Result Value (Displacement) Versus Result Value
(Stress) from the Cantilever Beam’s Nodes as Shown.
7
146
PART 6
Results Postprocessing
Graph of Results Versus Global Variable (Transient Style)
Displacement versus time results are used in this example.
1. From the Select Results form (left most icon) select the
Result Cases from the first listbox. You must select more than one Result Case. Use the Select button if necessary or turn OFF the Abbreviate Subcases toggle.
2. The Y-axis should be set to Result values.
3. Select the Y-axis result quantity (displacement) from the
Select Y Result listbox.
4. (Optional) Set the result Quantity if necessary (to
Magnitude for this example).
5. (Optional) If more than one layer exists for these results, also select the layer you wish to plot.
6. Set the X-axis to Global Variable (time). If more than one global variable exists, select the one you want to plot against.
7. Use the Target Entities form to select nodes as target entities. Graphically select the nodes from the screen after setting the target entities to nodes. You can pick as many nodes as you wish or as few as one. Too many will clutter the plot. One curve will result for each target entity selected for transient style plots.
8. (Optional) Use the Display Attributes form to make any changes to the display attributes of the plot.
9. Press the Apply button.
Y: Result
Quantity: Magnitude sition...(NON-LAYERED
X:Global Variable
Variable:
Time
Apply
Time (Seconds)
Figure 8-3 Result Value (Displacement) Versus Global Variable
(Time) for Various Nodes of a Model (Transient Results).
CHAPTER 8
Graph (XY) Plots
147
Add Curve to Existing Graph
1. Follow any previous example to create a graph. For the sake of this example we will assume that another curve should be
at another node. So first follow the
Graph of Results Versus Global Variable
2. Go to Display Attributes.
3. Turn ON the Append Curves toggle.
4. Go to Target Entities and select a new node to create a transient curve from.
5. Press the Apply button. The new curve will be added to the existing XY Window retaining all previously created curves. All curves will be associated with the same Graph plot. In this case the default_Graph since we did not specifically give it a name.
Append Curves in XY Win
Apply
7
7
148
PART 6
Results Postprocessing
Graph of Global Variable Versus Global Variable
This example uses design optimization results to plot design variables versus design iteration.
1. From the Select Results form (left most icon) select the
Result Cases from the first listbox. You must select more than one or you will only get one data point for your graph.
2. The Y-axis value should be set to Global Variable.
Y:Global Variable
3. Select the Y-axis global variable from the Variable pulldown menu.
Variable:Design Var 1
4. Set the X-axis to Global Variable.
X:Global Variable
5. Select X-axis global variable from the Variable pulldown menu.
6. No Target Entities need to be selected for this type of plot.
7. (Optional) Use the Display Attributes form to make any changes to the display attributes of the plot.
8. Press the Apply button.
The plot below shows four curves. To create this the
Append Curves in XY Window toggle was turned ON so as to create only one XY window with multiple curves. See the
Apply
Design Iteration
Figure 8-4 Four Plots of Global Variable (Design Variables)
Versus Global Variable (Design Iteration).
CHAPTER 8
Graph (XY) Plots
149
Graph of Beam or Edge Results
The moment along the length of a beam (or element edges) was used for this example.
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. The Y-axis should be set to Result values.
3. Select the Y-axis result quantity (Bar or Shell Forces,
Translational or Rotational) from the Select Y Result listbox.
4. (Optional) Set the result Quantity if necessary (to Y
Component for this example).
5. If more than one layer exists for these results, also select the layer you wish to plot.
6. Set the X-axis to Beams (It could also be set to Path Length).
Y: sition...(NON-LAYERED
Y:
Result
Beams
7. Go to Target Entities.
8. Select the beams or element edges as target entities.
Graphically select them from the screen. The target entities should be set to Path. The entity display attributes should be
Edges/Beams.
Select Path Edge/Beam
Additional Display Cont dges/Beams
9. (Optional) Specify how many points (result locations) should be used per curve segment in the Points Per Segment databox. This will determine how many data points will make up the resulting graph.
Points Per Segment
3
10. (Optional) Use the Display Attributes form to make any changes to the display attributes of the plot.
11. Press the Apply button.
Apply
7
Path Distance
Figure 8-5 Result Value (Moment) Along a Set of Beams.
7
150
PART 6
Results Postprocessing
Graph of a Results Value Along an Arbitrary Path
An arbitrary path was defined by a curve created in the plane of the elements defining a cantilever beam for this example.
1. From the Select Results form (left most icon) select the
Result Case from the first listbox.
2. The Y-axis should be set to Result values.
3. Select the Y-axis result quantity (Displacements) from the
Select Y Result listbox.
Y:
Result
4. Set the result Quantity if necessary (to Magnitude for this example).
5. If more than one layer exists for these results, also select the layer you wish to plot.
6. Set the X-axis to Path Length.
Quantity: Magnitude sition...(NON-LAYERED
Y: Beams
7. Use the Target Entities form to select the curve or curves as target entities.
8. Graphically select them from the screen. The target entities should be set to Path. The entity display attributes should be
Curves.
Select Path Curves
Additional Display Cont
Curves
9. (Optional) Set the Points Per Segment up to a reasonable number to create points in between the end points of the curve(s). If set to one (1), only results at the end points of the curve will be plotted.
Points Per Segment
3
10. (Optional) Use the Display Attributes form to make any changes to the display attributes of the plot.
11. Press the Apply button.
Apply
Path Distance
Figure 8-6 Result Value (Displacement) Along an Arbitrary Path
(Defined by a Curve) as Shown on the Cantilever Beam.
CHAPTER 8
Graph (XY) Plots
151
Save a Graph Plot
1. Set up the graph plot as explained in the above examples but do not press the Apply button.
2. Before pressing the Apply button to create a plot or animation, press the Plot Options icon button (fourth button from the left).
3. Type a name in the Save Graph Plot As databox.
Save Graph Plot As: myGraph
4. Then press the Apply button.
Apply
Modify a Plot
1. Set the Action to Modify with the Object set to Graph.
2. Select an existing graph plot from the Existing Graph Plots
Existing Graph Plots...
listbox.
3. Change results, target entities, display attributes, plot options, or other attributes as required.
4. Press the Apply button at any time to see the results of your modifications.
Apply
7
Frequency (Hz)
Figure 8-7 Result Value (Displacement) Versus
Global Variable (Frequency) of Different Damping Values.
7
152
PART 6
Results Postprocessing
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
9
Animation
■
■
■
■
■
8
154
PART 6
Results Postprocessing
9.1
Overview
Result animations are an integral part of understanding the behavior of a structure, especially those subjected to dynamic forces. Animations in MSC.Patran are set up in a variety of ways.
Most plots, once created, can be animated. Or they can be animated at creation time. To successfully create an animation it is important to first understand how to create a plot. For an overview of how the Results Application works please see
To specifically create an animation of a given plot type at creation time, simply turn ON the
Animate button with the Object set to the desired plot type. The general steps to take when creating an animation at plot creation time are :
Action:
Object:
Create
Deformation
Step 1:
Set the Action to Create and select an Object (the plot type) from the Results application form.
Select Result Case(s)
Load Case 1, Static Subcase
Step 2:
Select a Result Case from the form for animation of static results. Select multiple Results Case if a transient animation is desired.
Select Deformation Result
Applied Loads, Translational
Displacements, Translational
Displacements, Rotational
Step 3:
Select a result type from the form.
Step 4:
Turn ON the Animate toggle.
Animate
-Apply-
Reset All
Step 6:
Press the Apply button on the bottom of the form. Animation frames will be created and animation will begin.
Step 5:
Change any target entities or other attributes and options if desired (optional).
Note:
Animation options are set by pressing this button icon. Detail on animation options and animation control can be found in
There are two aspects of animation: setting up the animation and controlling the animation once the animation frames have been created. For most basic animations, the default settings will be appropriate. However full control is given to the user to change animation options.
CHAPTER 9
Animation
155
Animation options for any given plot type is controlled from the Animation Options form which is accessible by pressing the right most button icon on the Results
Application form when the Object is set to a plot type. These options control things such as the number of frames to be generated, the animation method (modal, ramped, global variable), starting and ending values, 2D or 3D animation and interpolation methods. All settings are saved with a plot when it is created whether animation has been enabled or not. An
explanation of these settings is given in
Once an animation is in progress or the frames are being created, a form appears to control the animation. Control is given over such things as stopping and starting, pausing, stepping, speeding up and slowing down the animation. More detailed explanation of animation control
It is possible to save any result plots to the database with a specific name. In fact all plots are saved to the database with default names if none is given. Any plot that has already been created and saved to the database can be animated even though it was not animated when it was created.
All attributes of that plot have been saved such as the result or results associated with it, its display properties, target display entities, and other options. Any animation attributes given to a plot is only active as long as the plot is posted. They are not saved in the database. Animation of existing plots is done by setting the object in the Results application to Animation and then selecting the plots to animate and those to remain static. This is explained in detail in the next section.
8
8
156
PART 6
Results Postprocessing
9.2
Animation Options
There are two aspects of animation: selecting animation options before animation actually begins, and controlling the animation once plots are animating. This is the most general display of the Animation Options form.
Action:
Object:
Results
Create
Deformation
Animation Method:
Global Variable
Select Global Variable
LOAD CASE INDEX
Time
Increment
Min: 0.1
Max: 1.
Start Value:
End Value:
Apply
0.1
1.0
Animation Graphics
2D
3D
Preview
MPEG
VRML (Max 120 Frames)
Default Window Size
Number of Frames:
Interpolation:
Animate
8
Linear
Reset
Press Apply to create the animation. Be sure, however that you have turned on the
Animate button on the main form when selecting results. Otherwise no animation will be created. This form is for simply setting animation options.
Animations are initially set up using the Animation Options form which is selectable for most plot types by selecting the right most icon on the Results application form. Intelligent default options have been set making it unnecessary to enter this area unless options need to be changed.
Several animation types are available. Modal animation allows animations from +MAX (positive maximum value) to
-MAX (negative maximum value), whereas Ramped animation only ranges from ZERO to +MAX. These are the only options available for animating static results or results from a single results case (deformed plots, mode shapes, etc.). For transient data the Global Variable method is also available. You must select a global variable when animating transient data and you must have selected more than one subcase (time step) from a results case for this method to be
For transient animation or animation of multiple results cases you must select a global variable and specify a starting value and ending value. For transient data the global variable is generally time. When the number of frames to plot is not the same as the number of time steps then interpolation is used to create the missing frames. The interpolation method can be controlled at the bottom of this form.
2D animation allows for animation frames to be created only in a
2D plane. This simply means that dynamic rotation with the mouse is not possible without recreating all the animation frames again. 3D animation allows for dynamic rotation with the mouse. The advantage of 2D over 3D animation is speed, although this is highly hardware and model size dependent.
Preview will step through each frame and quit. This is best used for transient animations. MPEG or VRML allows for output of animations to these standard formats, in addition to the display in the viewport. See
File>Images
(p. 197) in the MSC.Patran
Reference Manual, Part 1: Basic Functions.
Controls the window size of image output when the
MPEG or VMRL outputs are requested.Turning this toggle ON sets the output file window size to an acceptable size for most image view programs.
Enter the number of frames for the animation to build. The default is 7. There is no current imposed limit to the number of frames that may be used. The more frames used, the smoother the animation will appear, however practical limits such as available memory and model size will quickly dictate the limit. If VRML output is requested, then the maximum number of frames allowed is 120.
CHAPTER 9
Animation
157
Animation Interpolation.
To create the specified number of frames for any animation, the program will do interpolation of the data because in most cases there will not be a one to one correspondence of frames to number of results cases. The default is to use Linear interpolation.
The interpolation method has no effect on the animation of static data (mode shapes, deformed plots). Each frame is determined using a simple harmonic or linear scale factor multiplied by the given static result.
For transient animation this is not the case. The interpolation method is used to determine how results are calculated for frames which do not have exact results present. During transient animation, the selected global variable is scaled linearly from its starting to ending value, evenly progressing between each animation frame. If the Load Case Index is chosen, then a dummy variable is assigned to each specified loadcase (1.0-n) and it is used as the interpolation basis (the independent variable). Once a global variable value is determined from each frame, the result values are then calculated based on the available results specified for the animation.
The following is a table of interpolation methods along with their descriptions:
Linear
Action
Closest Value
None
Description
This is the default interpolation function. The results for a given frame are determined using linear interpolation which performs a weighted average of the two closest results cases to the current frame.
No interpolation is performed. Only results found in the analysis are used. The closest results values associated to the current global variable are used for frame creation.
No interpolation is performed. Only results found in the analysis are used. The None interpolator will simply repeat the last usable data to fill the excess frames.
8
8
158
PART 6
Results Postprocessing
9.3
Animation Control
The Animation Control form automatically appears when the animation toggle has been turned
ON after the Apply button has been pressed to create the animation.
Pause/Stop or Restart the animation currently running. The animation must be paused to enable any capability other than the start and end frame values.
Animation Control
Pause Animation
Adjust the slidebar or enter a value for the current frame to display a paused animation. Adjusting the slidebar or entering a value in the databox will update the display accordingly.
1 15
1
Frame Displayed If an animation is currently paused, click this button to step through the animation frame-by-frame using the current method.
Advance Frame
Animation Sequence
Cycle
◆
Bounce
Select a method for displaying the current animation.
Cycle will display the animation frames 1:n, 1:n,...
Bounce will display the frames 1:n:1:n... Bounce gives a much more continuous looking animation for the ramped method. For the modal method, Cycle and Bounce look much the same. Transient animations are more realistic in Cycle mode.
1 14
1
Starting Frame
2 15
15
Ending Frame
Slow
Animation Speed
Stop Animation
Fast
Adjust the slidebars to set a value, or enter a value in the appropriate databox, for the Starting Frame and Ending
Frame of the animation currently running. Changing these values will skip the display of all the frames above or below the entered values, respectively.
Adjusts the speed at which the animation frames are played back.
Ends an animation and clears it from the screen. Other methods of stopping an animation are to press the Abort or Cleanup icons (the hand or broom respectively) on the main MSC.Patran form, close the database down or quit from MSC.Patran.
The Animation Control form will close down once Stop Animation is pressed or the animation is stopped.
CHAPTER 9
Animation
159
9.4
Animating Existing Plots
The following form and explanation show how to create animations of existing plots. All plots are saved in the database with their corresponding attributes, results, and other options associated with them. It is then a simple matter of turning ON or OFF the animation of these plots via this form. Set the Action to Create and the Object to Animation in the main Results application formIt is possible to record these animations using the new MPEG output (See
MPEG Images Output
(p. 199) in the MSC.Patran Reference Manual, Part 1: Basic Functions). The
File Images Form can be opened to allow recording of the MPEG file during animation playback.
Results
Action:
Object:
Create
Animation
Method:
2D Graphics
Plots to Animate
None-DEF_default_Deformation
Ramp-FRI_default_Fringe
Modal-TEN_default_Tensor
GV-VEC_default_Vector
The Method of animation can be in software (2D) or hardware
(3D) mode. The main difference between these two are that hardware allows for dynamic rotation while animating in software does not. Additionally, a Preview method can be used to display each frame successively with no animation.
All posted plots appear in this listbox. One by one you will indicate which to animate and how. This is done by first selecting a plot. Its animation attributes will appear below. The animation attributes are those that were originally set up when creating the plot and can range from None to Ramped to Modal to Global Variable (GV). Note that the animation attribute is indicated next to the plot name for easy reference.
Animate By: Global Variable
Select Global Variable
LOAD CASE INDEX
Time
These animation attributes are explained in
.
8
Min: 0.
Start Value:
0.0
Max: 2.
End Value:
2.0
Number of Frames:
7
Interpolation
Linear
-Apply-
Specify the number of frames to be created for the animation.
There is no limit, however memory and computer speed may quickly determine the practical limit. Interpolation methods only apply to transient animations when multiple results cases have been selected. They are explained in
Creates the animation of the specified plots. The animation control form will appear showing the progress of the creation of the animation frames. This form is explained in
8
160
PART 6
Results Postprocessing
The following table describes in more detail the different animation attributes that can be set when setting up animation of several existing plots.
Table 9-1 Animation Attributes
Option Description
None
Modal
Ramped
If no animation has been initially set up when the plot was created, this is the animation attribute that it will have. None indicates that this plot will not animate. If you do not wish for a plot to animate, yet it is posted to the viewport, then this attribute must be set to None. The word None- will be placed next to the plot name to indicate that no animation will occur for the plot.
Setting a plot to Modal indicates that you want a modal style animation.
This is common for modal analysis results. Modal style animations oscillate from the maximum results value to the negative of the maximum value, or in other words, it is like a fully reversed loading situation that oscillates like a sine function. When specifying a modal animation you can also set an angle offset. This sets up a phase shift in your animation. For example if you want to turn a sine wave oscillation into a cosine oscillation, use an offset angle of 90 degrees. The word
Modal- will be placed next to the plot name to indicate that no animation will occur for the plot.
A ramped style animation is good for animating statically loaded structures. The oscillation will proceed in a ramped form from a scale of zero to the maximum result value over the number of frames indicated.
That is it will deform or animate from its position in rest to its fully deformed or stresses state (for deformation plots). The word Ramp- will be placed next to the plot name to indicate that no animation will occur for the plot.
Global Variable
This animation attribute can only be assigned to plots that have multiple
Result Cases assigned to it in the case of transient animation. In this case you must indicate which global variable to use, and its start and end values. Animation frames will then be created from the results based on an interpolation scheme selected by the user. By default linear interpolation is used. This is the only animation attribute that uses interpolation. All others (Modal and Ramped) simply use linear scaling since only one Result Case is ever involved. See
(p. 157) for more detail. The word GV- will be placed next
to the plot name to indicate that no animation will occur for the plot.
CHAPTER 9
Animation
161
9.5
Examples of Usage
The following are the typical scenarios for creating animations when creating a new plot or from existing plots.
Create an Animation at Plot Creation Time (Static or Transient)
1. Decide what type of plot you wish to animate: deformation, fringe, vector, tensor, etc. Set the Action to Create and
Object and/or Method accordingly.
Object:
2. Select the Results Case(s) from the first listbox. Select one
Results Case for an animation of a static result. Select multiple Result Cases for a transient style animation. You may wish to use the Select Subcases button icon to more easily filter multiple Result Cases.
3. Turn ON the Animate toggle. If an Animate toggle is not present on the main Select Results form for the desired
Object, then that plot type does not support animation.
4. (Optional) Set any other options such as target entities, display attributes, and plot options by changing the form and subsequent settings with the button icons at the top of the form just below the Action and Object menus.
5. Modal style animations are the default for static, single right most button icon (Animation Options) to select a global variable (time, frequency, etc.). This is necessary for determining proper interpolation of results for each animation frame.
6. Press the Apply button.
If the Animate toggle was not turned ON, then no animation will result. Instead the Results application will simply create a static plot of the selected Result Case or a maximum plot of multiple Result Cases.
Fringe
Animate
Apply
8
Z
Y
X
Figure 9-1 Modal Animation of Cantilever Plate
8
162
PART 6
Results Postprocessing
Create an Animation from Existing Plots
1. First make sure that the plots you wish to animate are posted to the current viewport. This is done by setting the
Action to Post and the Object to Plots and selecting the desired plots from the listbox and pressing Apply.
Action:
Object:
2. Set the Action to Create and the Method to Animation.
Action:
Object:
Post
Plots
Create
Animation
3. If necessary, set the Method to software (2D) or hardware
(3D) mode (hardware mode allows for dynamic rotation while animating in software does not). Speed performance may also differ between the two methods.
Method:
2D Graphics
4. From the Plots to Animate listbox, select a plot that you wish to animate.
5. Change the Animate By option pulldown menu to the desired animation attribute which can either be None,
Modal, Ramped, or by Global Variable. Global Variable is only selectable if the plot has been set up with multiple
Result Cases for a transient style animation.
Animate by: Modal
6. (Optional) You may need to change other options such as the Angle Offset for modal animations or global variable information for transient animations.
7. Repeat steps
for each plot you want to animate (to
not animate, but still plot, set the attribute to None).
8. (Optional) Set any other animation options on this form as
Number of Frames:
desired such as the number of frames to create and interpolation method for transient animations.
Interpolation:Linear
15
9. Press the Apply button.
Any combinations of animation types can be combined together. An example of simultaneously animated plots is shown in
Apply
In general, with the exception of the number of frames or other animation options set on this form, all display attributes and other options associated with the plots to be animated will be retained.
Z
Y
X
Figure 9-2 Simultaneous Animation of a
Bending Mode (Magenta) and a Torsional Mode (Red).
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
10
Reports
■
■
■
■
■
9
164
PART 6
Results Postprocessing
10.1
Overview
The Report object in the Results application allows for creation of text reports of any result that has been imported into the database or created by any other means such as derivations or combinations from other results quantities.
The Report application works much the same way as any other plot type in the Results application with the only real difference being that a text report will be created as opposed to a graphical display. For an overview of how the Results application works see
There is only a slight difference between Create and Modify. The main difference is that Create must be used to make a report and Modify is used to change an existing one. If you try to modify an existing report with Create you will be asked for overwrite permission whereas Modify assumes that the action is desired, so no overwrite permission is requested.
Toggles the form to select results for reports. This is the default mode of the
Report form.
To create or modify a report, follow these general instructions:
1. Set the Action to Create, the Object to Report and the Method to the desired type. This depends on whether the report is to be displayed in the invoking window or written to a file. Preview will display the report in the invoking window, Overwrite File will create a new file or overwrite an existing one by the same name. Append File will append to an existing file.
2. Select a Result Case or multiple Result Cases from the Select Result
Case(s) listbox. The results that appear in the listbox can be filtered.
See
3. Select a result to report from the Select Report Result listbox.
4. If multiple layers exist for the selected result, select the layer positions that you wish to include in the report using the Select
Positions listbox.
5. Specify the quantities associated with the selected result from the
Select Quantities listbox. Some logical defaults are usually selected such as the components of a stress tensor or displacement vector.
For explanations of derived results such as von Mises see
CHAPTER 10
Reports
165
6. At this point you could press the Apply button to create the report.
By default the report will be directed to the invoking window with the Method set to Preview. However, you may wish to direct the report to a file and/or change the format of the printed report using the Format button and its subordinate form. See
7. If directing the report to a file, make sure to set the Method to the appropriate selection, either Overwrite or Append mode. Specify a filename if not in Preview mode or accept the default. The filename can be changed under Display Attributes. Sorting options are also found there.
8. If you wish to report results for just a portion of the model, change the target entities for which the report is to be written by pressing
the Target Entities button icon. See
9. If other options are necessary to tailor the results report, such as coordinate transformation, averaging and extrapolation methods, sorting options, results filter values, or a scale factor then use the
10. Press the Apply button to create the report.
Apply
Selected Quantities.
The following table explains the different quantities that can be included in a report. For a more detailed explanation of derived quantities see
Quantity
Scalar Value
NSHAPE
Loadcase ID
Subcase ID
Layer ID
X/Y/Z Location
CID
Description
When a scalar result has been selected for a report this is the generic name of the quantity. It is selected by default when a scalar value has been chosen for a report.
This is a variable that is used with elemental data and outputs an integer value indicating the type of element the result is associated with (Bar=2, Tri=3, Quad=4, Tet=5, Pyr=6, Wed=7, Hex=8). This variable is generally only used when outputting a scalar elemental
MSC.Patran results file. See
Create a MSC.Patran .els Formatted
This is the internal Load Case or Result Case ID that is associated with the result quantity. Generally this information is output with report summaries.
This is the internal subcase ID associated with the result quantity.
Generally this information is output with report summaries.
This is the internal layer ID associated with the result quantity.
Generally this information is output with report summaries.
The X, Y, or Z coordinate location in the MSC.Patran global coordinate system.
The coordinate system ID that the reported results are in.
9
9
166
PART 6
Results Postprocessing
Quantity
Material ID
Material Name
Property ID
Property Name
ACID
Magnitude
X/Y/Z
XY/YZ/ZX
Component von Mises
Max/Mid/Min
Principal
Hydrostatic
1st, 2nd, 3rd
Invariants
Tresca
Max Shear
Octahedral
Description
The internal material ID of the region of interest (zero if none exists).
The material name currently assigned to the region of interest. If none exists then “ErrErr” will be reported.
The internal property ID of the region of interest (zero if none exists).
The property name currently assigned to the region of interest. If none exists then “ErrErr” will be reported.
The analysis coordinate system attached to the entity ID (node) which is recovered from the entity record in the database. Results from the analysis code are generated in the ACID system.
The magnitude derived from a vector quantity.
The X, Y, or Z components of a vector quantity or the X, Y, Z, XY, YZ, or ZX components of a tensor quantity.
von Mises stress derived from a stress tensor.
The maximum, intermediate or minimum principals derived from a tensor.
The Hydrostatic stress derived from a stress tensor.
The 1st, 2nd, and 3rd invariant stresses derived from a stress tensor.
Tresca stress derived from a stress tensor.
Maximum shear stress derived from a stress tensor.
Octahedral stress derived from a stress tensor.
CHAPTER 10
Reports
167
The following quantities are also reported dependent on the type of result selected and target entities.
Quantity
Entity ID
Node ID
Position ID
Description
This is the ID of the Node or Element being reported. This Entity ID will always appear. The only control you have over this, is in which
When element nodal data is being reported this is a node number connected to the element (Entity ID) for which results are being reported. For element nodal data, these node IDs appear automatically so you may distinguish which element result row belongs to which node. Only the column in which the node ID is
When element Gaussian data is being reported this is a position ID of the element (Entity ID) for which results are being reported. For element Gaussian data, these position IDs appear automatically so you may distinguish which element result row belongs to which position. Only the column in which the position ID is displayed can
(p. 170). Element position number
are internal IDs which are generally meaningless to users. However -
999 signifies centroidal data, and 0, -1, -2, ... signifies internal node
(coincident not the nodes) locations. Actual Gauss points will have their own internal IDs.
9
9
168
PART 6
Results Postprocessing
10.2
Target Entities
Reports can be created for various model entities. By default reports are created for everything displayed in the current viewport. To change target entity selection for results reporting, press the Target Entities icon with the Object set to Report.
Toggles the form to select target entities for report generation.
The following is a description of all target entities and target entity attributes.
Entity Description
Current Viewport
By default reports are created for all finite element entities displayed in the currently active viewport.
Nodes
Individual nodes may be selected for which to create a report. You may type in any node numbers manually or by selecting them graphically from the screen. Be sure to include the word Node in front of the IDs you type in manually, (i.e., Node 1 5 55 100 etc.). To select all nodes use the syntax “Node 1:#.”
Elements
Groups
Individual elements may be selected for which to create a report. You may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.). To select all elements use the syntax “Elem 1:#.”
Reports can be limited to only selected groups. A listbox will appear allowing selection of the groups for generating a report. Only for entities belonging to those groups selected will a report be generated.
Materials
Properties
Element Types
Reports can be targeted at only those finite elements which have certain material properties assigned to them. A listbox will appear allowing selection of the materials for whose entities will be reported
Reports can be targeted at only those finite elements which have certain element properties assigned to them. A listbox will appear allowing selection of the properties for whose entities will be reported.
Reports can be limited to only certain element types also.
CHAPTER 10
Reports
169
In addition to selecting the target entities from which to generate a report, it is also necessary in some cases to specify the entity attributes to further define what data is to be reported. For target entities in the Current Viewport, Elements, Groups, Materials, Properties, and Element Types it is necessary to specify where to report the values.
Attribute Description
Nodes
Element
Centroids
Results data will be reported at the nodes only. This is most appropriate for nodal type data. For elemental type data, the results will be extrapolated to and averaged at the nodes for reporting single values at each node of the target entities.
Results data will be reported at the element centroids. This is most appropriate for element centroidal type data. For nodal data, the values will be averaged from each contributing node and reported as a single value at the center of each element of the target entities. The same is true for elemental data with more than one value associated with each element
(element nodal data or element Gauss data).
Element Nodes
Results data will be reported at the nodes for each element in the target entities. This is most appropriate for element nodal data where results for every element exist at the nodes. This is not appropriate for nodal type data at all. For element centroidal data and other element data (such as at gauss points) the results will be extrapolated to the nodes. Results are therefore reported by element followed by associated nodal results for the given element.
Element All
Data
Results data will be reported as is. This is most appropriate for element results at gauss points. The data will be left as is. This is true also for element nodal and element centroidal results but no indication of node numbers will be given, simply element positions as stored internally in the database. This is inappropriate for nodal type data.
9
Important:
Once a target entity has been selected, it will remain the target entity for the report until the user physically changes it.
9
170
PART 6
Results Postprocessing
10.3
Display Attributes
Result reports can be formatted in a variety of ways and with many options.
Toggles the form to set display attributes and formatting options of reports.
Below are descriptions for all the fields and settings for formatting text reports.
Item Description
File/File
Name
Specify a file name to direct the report to. You can only specify a file name if the
Method has been set to Overwrite or Append File. A file browser is also available if you press the File button to select an existing file. The default filename is
patran.prt.
This can be overridden with a settings.pcl
parameter: pref_env_set_string(“result_capture_filename”,“patran.prt”)
See
The settings.pcl file
(p. 41) in the MSC.Patran Reference Manual, Part 1:
Basic Functions.
Format...
A subordinate form will appear to allow for report formatting. This is explained below in
Sorting
Options
A subordinate form will appear to allow for selection of sorting options. This is
Report
Type
A full report includes summary and data. Only summary information such as load case and max/min values can be requested as well as data only with no summary information.
Report Format.
Below are descriptions for all the fields and settings for formatting text reports.
Item
File Width
Lines/Page
Top Margin
Left Margin
Pagination
Page Number
Table 10-1 Results File Format Options
Description
Sets the number of characters that can fit in the width of a page including spaces. The default is 128 characters.
Sets the number of lines per page. The default is 52 lines per page.
Sets the number of lines used to form a top margin. The bottom margin is set by the number of Lines/Page.
Sets the number of characters used to make a left margin. The right margin is set by the File Width.
If you wish to use pagination turn this toggle ON. The Page Number setting will appear to set the beginning page number. No footer or header information will be printed.
Set the beginning page number with this option. This databox only appears if Pagination has been turned ON.
CHAPTER 10
Reports
171
Edit
Item
Alignment
Title/Header/Footer
Text Format
Display Column
Labels
Input Column/
Label/Format
Column
Column Label
Value Format
Order Columns
Table 10-1 Results File Format Options (continued)
Description
This is an option menu for editing the Title, Footer, or Header. No
Footer or Header is allowed if pagination is OFF. This text box below this menu will update to allow for editing of the selected text.
Alignment of the report can be from the left margin, right margin or the report can be centered.
This textbox allows for inclusion and modification of a Title, Header or Footer. Which is set for editing is determined by the Edit option menu above this text box. You may place a %I% in any of these text boxes to include the page number if Pagination has been turned ON.
You may also include a %rN% for including additional lines after.
These formatting characters are explained in .
This toggle will turn on or off printing of the Column labels. The column labels are the middle column of the spreadsheet shown on the Results File Format form.
This is a databox that becomes active to allow for changes in the actual Column numbers, Column Labels, or Value Formats. Simply click on a cell in the spreadsheet that appears below this databox and the databox will become active to allow you to change the cells contents. If you wish to reorder the columns, change the column numbers using this mechanism and then press the Order Columns button to reorder their appearance in the actual spreadsheet. If no results have been selected before the Format form is opened, the spreadsheet will not appear below this databox.
This is the column number with its associated label and value format. If you wish to change this to a different column, simply click on this cell and enter the column number where you wish this label and its values to appear using the databox above. Press the Enter or
Return key to effect the change.
This is the label that appears above the column of results. By default it is the same as results quantities selected. To change a label, select the cell and then change the value in the databox above. Press the
Enter or Return key to effect the change.
Results formats are listed in this column. They specify how the actual results values will be formatted in the report. They consist of the format characters surrounded by percentage signs. To change one of these formats, click on the cell that contains the format to change and enter your changes in the databox above the spreadsheet. Press the Enter of Return key to effect the change. The different characters and combinations acceptable for these formats is
If you wish to reorder the columns once you have manually changed the column numbers in the spreadsheet then press this button.
9
9
172
PART 6
Results Postprocessing
Important:
The order in which the quantities are arranged in the spreadsheet of the Format form is dependent on the order in which you selected them from the Select
Quantities listbox. Select them from the list box in the order in which you wish them to appear in the report. Use the Control key for discontinuous selections.
Format Strings.
gives a description of output format strings used to convert integer, real, and
string data to a formatted output. It is necessary to use these strings in the Value Format column in the spreadsheet to specify how to format the results values in the report. Some of these formats can also be used in the Title, Header and Footer. The format string is a simple character string which contains both raw text to output, and format specifiers, enclosed by a set of percent characters, which control how data items are formatted and output. Upper case letters (I, F, E, etc.) are interpreted literally and lower case letters are to be substituted with the appropriate values.
To change a value format simply click the mouse button with the cursor in the cell whose format you wish to change. Then in the Input databox above the spreadsheet change the value format to what you want and then press the Return or Enter key.
%%
Table 10-2 Value Format Strings for Formatting Text Report Numbers
Format
%Im%
%Fm.n%
Description
The simplest form of format specifier is a double percent to produce a single percent in the final output. Used if you want a percent character in the Title, Header or Footer.
Integer (I) specifier. This format specifier takes an integer value such as a node or element (entity) ID or other integer result for formatting. The value of “m” is the minimum number of characters to produce from the format. If “m” is omitted, then the exact number of characters necessary to hold the integer is used. The exact format produced is an optional minus sign followed by one or more digits. The default for integer data is %I6%.
Fixed (F) float specifier. This format specifier takes a real results value for formatting in fixed point notation. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters necessary to hold the conversion is used.
The value of n is the number of decimal digits to produce. If omitted, then all significant digits will be produced. The exact format produced is an optional minus sign followed by zero or more digits, a decimal point, and zero or more digits. At least one digit will precede or follow the decimal point. The default for real data is %F12.6%.
CHAPTER 10
Reports
173
Table 10-2 Value Format Strings for Formatting Text Report Numbers (continued)
Format
%Em.n.p%
%Gm.n.p%
%Sm%
%rN%
Description
Exponential (E) float specifier. This format specifier takes a real value for formatting in scientific exponential notation. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters necessary to hold the conversion is used. The value of n is the number of decimal digits to produce. If omitted, then all significant digits will be produced. The value of p is the number of digits to display before the decimal point, and defaults to one. If zero is specified, then a single zero precedes the decimal point. The exact format produced is an optional minus sign followed by zero or more digits, a decimal point, zero or more digits, a capital E, a plus or minus sign, and two decimal digits. At least one digit will precede or follow the decimal point. The default value for read data is the F format.
General (G) float specifier. This format specifier takes a real value for formatting in either F or E format. The format used depends on the value of the number to convert. In general, if the exponent is small, the F format will be used, otherwise the E format is used. See the descriptions of the F and E formats.
String (S) specifier. This format specifier takes the next string value from the character data array for formatting. The value of m is the minimum number of characters to produce from the format. If m is omitted, then the exact number of characters in the string is used. The default value for string data is %S32%.
New (N) line specifier. This format specifier causes a new line to be started. The previous line is output as is, and formatting starts at column one of the new line. The value of r is a repeat count for skipping multiple lines. If output is to a string, then new line characters will be written to the string. This is used in the Title, Header and Footer text.
Variables.
Variables can be placed in titles, footers, or headers of reports. The variables available are shown in the table below. Be sure to place the $ symbol in front of the variable otherwise it will not be recognized as a variable.
Format
$LC_NAME
$SC_NAME
$PRES_NAME
$SRES_NAME
$LYR_NAME
$DATE
Table 10-3 Value Format Strings for Formatting Text Report Numbers
Description
This is the Result Case (load case) name.
This is the subcase name.
This is the primary result name.
This is the secondary result name.
This is the result layer name.
The current date and time in the format dd-mmm-yy hh:mm:ss.
9
9
174
PART 6
Results Postprocessing
Table 10-3 Value Format Strings for Formatting Text Report Numbers (continued)
Format
$PAGE
$NNODES
$MAXNOD
$DEFMAX
$NDMAX
$NWIDTH
$DATA_TITLE
$PRODUCT
$DB_NAME
$JOB_NAME
$CODE_NAME
$GV:<name>
$LEFT
Description
The current report page number.
The number of nodes in the report. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case. Typically used to create MSC.Patran nodal (nod) result files.
The highest ID of a node in the file. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case. Typically used to create MSC.Patran nodal (nod) result files.
The maximum value encountered within the file. Variable is printed in
E15.6 format if left aligned. Valid for nodal report only, sorted by Result
Case. Typically used to create MSC.Patran nodal (nod) result files.
The ID of the node with the maximum value. Variable is printed in I9 format if left aligned. Valid for nodal report only, sorted by Result Case.
Typically used to create MSC.Patran nodal (nod) result files.
The number of columns in the file. This will be the number of results quantities output to the report. Note that the Entity Id which is the first column of most reports by default is not included in NWIDTH. It is actually the number of columns of real, floating point data. Typically this is used to create MSC.Patran nodal (nod) and elemental (els) result files.
The register title. You must use the built in function res_data_title() to set a title for your register. Once this title is set, then it will show up when you use $DATA_TITLE. See the
Data Register Definition
Functions
(p. 1139) in the PCL Reference Manual, Volume 1: Function
Descriptions.
The MSC.Patran product/version.
The name of the current database.
The name of the analysis job.
The name of the analysis code as set under Preferences/Analysis.
The name and value of an associated global variable such as time, frequency, eigenvector, etc. If a global variable is one word then all that is needed is to specify that global variable after the colon, i.e., $GV:Time.
However, if a global variable name has a space in it or, that is, consists of more than one word, you must surround the name with single quotes, i.e., $GV:’Design Cycle.’ Failing to do this will results in the variable picking up only the first word and will not find the correct global variable and will report garbage. Using this variable in the header and footer when multiple results cases (multiple GVs) will only use the first global variable encountered.
Aligns the current line of text to the left, overriding the global page alignment.
CHAPTER 10
Reports
175
Table 10-3 Value Format Strings for Formatting Text Report Numbers (continued)
Format
$MIDDLE
$RIGHT
Description
Aligns the current line of text to the middle, overriding the global page alignment.
Aligns the current line of text to the right, overriding the global page alignment.
Sorting Options.
Results can be sorted in a report and sorting is controlled via this form which is available from the Report Options form by pressing the Sorting Options button.
Sorting Options
Sort Order
Ascending
Sort By
Algebraic Value
Absolute Value
Sort Data By
Entity ID
X Component
Y Component
Z Component
XY Component
YZ Component
Descending
Results can be sorted in Ascending (from smallest to largest) or Descending order. Ascending order is the default.
Sorting can be done by comparing Algebraic Values which considers the sign of a value. A negative value will be treated as less than a positive number. Or the Absolute Value of the results can be used where sign is ignored, and the relative size in magnitude is considered in the sort.
This listbox displays the result entity by which the sort is based. By default sorting is always done and is based on the
Entity ID. This would be a node or element number in general.
Organized By:
Load Case Entity
OK
The report can be organized by either the Results Case (Load
Case) or by Entity. Load Case organization will report all results quantities for every entity for each load case. This is generally the way static results are reported and is the default.
However, for transient type data, it is sometimes easier to view a report in terms of the entities where results for a given Node
ID are reported for every time step (load case). Multiple Result
Cases must have been selected for this type of organization to be presented meaningfully.
9
9
176
PART 6
Results Postprocessing
10.4
Report Options
Reports have various options. Report options are accessible by pressing the Report Options selection button.
Toggles the form to select report options.
The following table describes the report plot options which can be modified:
Option Description
Coordinate
Transformations
Scale Factor
Filter Values
Vector and tensor results can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the MSC.Patran global system, a material coordinate system, element IJK coordinate system or the nodal
(analysis) coordinate system depending on the type of result (vector,
(p. 305) for a definition of each of
these coordinate systems. The default is no transformation, which will plot data in the coordinate frame as stored in the database. Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user. These can vary from node to node. Element data can be stored from the analysis code in any coordinate system. Note also that the analysis translators that import the results data into the can transform results. Check with the appropriate translator guide.
This scale factor has the effect of simply scaling the results up or down by the specified amount.
By specifying a filter value, a gate will be used to keep values below a maximum, above a minimum, between a certain range, or at the exclusion of certain values. The default is none. If filtering is used, only those elements which pass the filter gate will be reported.
Averaging Domain
For element based result quantities that must be displayed at nodes, an averaging domain must be used since more than one result will exist for each node. There is a contribution from each element attached to any particular node. By default all entities which contribute are used. Alternatively you can tell the Results application to only average results from those elements that share the same material or element property, are from the same target entities, or have the same element type. For more detail see
Averaging Method
The method in which certain results are determined can make a difference to the actual displayed plot. This is important when derived results from element based tensor or vector results are used such as
VonMises stress or Magnitude displacements, For instance if you average at the nodes first and then derive the desired quantity you may get a different answer than if you derive first and then average. It is left up to the user to decide which is correct. For more detail see
CHAPTER 10
Reports
177
Option
Extrapolation
Method
Complex No. as
Existing Reports
Save Report As:
Description
Many times element based results that are to be displayed at nodes exist at locations other than the nodes such as at integration points.
Various methods are available to the user to extrapolate these results out to the nodes. For more detail see
The Real component of a complex number is the default by which results will be reported. To force the report to use a different quantity such as Magnitude, Imaginary, Phase, or Angle, set this option pull down menu. This option will only be available if a complex result has been selected. It is not recommended to calculate invariants (e.g., von
Mises) from complex results because the phase is not accounted for.
This listbox displays all existing reports. You may select one of these from the listbox and all settings of that report including format attributes, target entities, option, and selected results will be restored.
This is an easy mechanism to help make many reports with the settings of an existing report without modifying the selected report much. When the Action is set to Modify, this listbox appears under the
Select Results display of the Results application form.
Reports can be saved by name and recalled later. These reports can be deleted as explained in
(p. 26) respectively. Once a report has
been created and named it retains all results, attributes, target entities, and options assigned to it. If no name is specified a default is created called default_Report
. As long as no name is specified, the default name will be overwritten each time a report is created.
Important:
Once report options have been selected, they will remain in effect for the report until the user physically changes them.
9
9
178
PART 6
Results Postprocessing
10.5
Examples of Usage
The following are some typical scenarios for usage of results reporting. These instructions assume that the Action is set to Create and the Object is set to Report and that results exist in the database unless otherwise specified.
Report of Displacement Data
1. Set the Method to Overwrite file. By default, a new file will be created called patran.prt.1
.
2. Select a Result Case from the first listbox.
Method: Overwrite File
3. Select a translational displacement result from the second listbox.
4. (Optional) Select X Component, Y Component, and Z
Component from the Select Quantities listbox. These may already be selected by default.
5. Press the Apply button accepting all format defaults and other option defaults.
The report should look somewhat similar to this:
MSC.Patran Version x.x 10/01/97 10:18:06 AM
Analysis Code: MSC.Nastran
Load Case: Load Case 1, Time=0.55
Result: Displacements, Translational- Layer (NON-LAYERED)
Entity: Node Vector
-Entity ID---X Component---Y Component---Z Component--
1 0.000251 0.000483 0.005989
2 0.000258 0.000488 0.006124
.
1467 0.000251 0.000455 0.006782
1468 0.000280 0.000501 0.006957
SUMMARY INFORMATION
--------------------------
Min/Max Values
-Source ID--Entity ID--X Component--
Min: 1 257 -0.001948
Max: 1 71 0.000882
-Source ID--Entity ID--Y Component--
Min: 1 257 -0.002525
Max: 1 55 0.001091
-Source ID--Entity ID--Z Component--
Min: 1 540 0.001625
Max: 1 257 0.009460
Apply
Figure 10-1 Report of Displacement Data with Summary
CHAPTER 10
Reports
179
Report of Transient Displacement Data
1. Set the Method to Overwrite file. By default, a new file will be created called patran.pr1
where database_name
is the name of the database. Change the name if you wish.
2. Select the Results Cases (time steps) from the first listbox.
Method: Overwrite File
3. Select a translational displacement result from the second listbox.
4. Select X Component, Y Component, and Z Component from the Select Quantities listbox. These may already be selected by default.
You could press the Apply button at this point and create a report similar to the previous example but repeated for each time step. However, it would be better to report the displacements for each time step together grouped together by entity ID.
5. Press the Display Attributes button icon (right most icon).
6. Open the Sorting Options form.
7. In the Sorting Options form change the Organized By switch from Load Case to Entity.
Sorting Options
Organized By:
Load Case Entity
8. Press the Apply button accepting all format defaults and other option defaults.
Apply
The report should look somewhat similar to
. Each line corresponds to the next time step for each entity ID. The title contains the names of each Result Case which is given a source
ID. From the source ID you can determine from the result data which source it is from.
9
9
180
PART 6
Results Postprocessing
MSC.Patran Version x.x 05/13/97 11:46:58 AM
Load Case: Load Case 1, Time=1.9
Result: Displacements, Translational- Layer (NON-LAYERED)
Entity: Node Vector
(First of 5 Sources)
Result Sources
-Source Id---Loadcase Name---------Subcase Name---------Layer Name----
1 Load Case 1 Time=1.8 (NON-LAYERED)
2 Load Case 1 Time=1.85 (NON-LAYERED)
3 Load Case 1 Time=1.9 (NON-LAYERED)
4 Load Case 1 Time=1.95 (NON-LAYERED)
5 Load Case 1 Time=2. (NON-LAYERED)
-Source ID--Entity ID--X Component---Y Component---Z Component--
1 1 0.000042 0.000774 0.005799
2 1 0.000774 0.000774 0.000774
3 1 0.005799 0.005799 0.005799
4 1 -0.000011 0.000775 0.005889
5 2 0.000775 0.000775 0.000775
.
1 320 -0.000077 0.000780 0.006008
2 320 0.000780 0.000780 0.000780
3 320 0.006008 0.006008 0.006008
4 320 0.000037 0.001000 0.007320
5 320 0.000595 0.000028 0.005629
.
Continues for every Entity ID
SUMMARY INFORMATION
_________________________
Min/Max Values
-Source ID--Entity ID--X Component--
Min: 1 556 -0.001338
Max: 5 556 0.000595
-Source ID--Entity ID--Y Component--
Min: 5 540 -0.002156
Max: 2 540 0.003511
-Source ID--Entity ID--Z Component--
Min: 5 540 0.001625
Max: 2 540 0.010750
Figure 10-2 Report of Transient Displacement Data.
CHAPTER 10
Reports
181
Create a MSC.Patran .nod Formatted File.
A MSC.Patran .nod file is a nodal based ASCII results file. The format of this file is:
Record 1:
Record 2:
Record 3:
Record 4:
TITLE
NNODES,MAXNOD,DEFMAX,NDMAX,NWIDTH (2I9 E15.6, 2I9)
SUBTITLE1
SUBTITLE2
Record 5 to n+4: NODID, (DATA(J), J=1, NWIDTH)
(80A1)
(80A1)
(80A1)
(I8, (5E13.7)) where:
TITLE
SUBTITLE1
SUBTITLE2
NNODES
MAXNOD
DEFMAX
NDMAX
NWIDTH
NODID
DATA
80A1 title stored in an 80 word real or integer array.
Same format as TITLE.
Same format as TITLE.
Number of nodes (integer).
Highest node ID number (integer).
Maximum absolute displacement (real).
ID of node where maximum displacement occurs (integer).
Number of columns after NODID for nodal information (integer).
Node ID number (integer).
Result quantities organized by column index (real).
1. Set the Method to Overwrite File. By default, a new file will
Method: Overwrite File
be created called patran.prt.1
. The name will be changed later.
2. In Select Results mode, select the Result Case from the first listbox.
3. Select a result from the second listbox.
4. (Optional) If necessary, select a layer. For this example, only one layer can be selected for a proper .
nod
file to be created.
5. Select the Quantities to output to the file. Only real (floating point data) quantities are valid for proper .
nod
files.
6. Go to Display Attributes.
Position...(at Z1)
7. Change the file name to patran.nod
.
8. Press the Format... button.
9. Set the File Width to 80.
Format
File Width: 80
9
9
182
PART 6
Results Postprocessing
10. Clear the Lines/Page, Top Margin, and Left Margin databox or put zeros.
11. Turn Pagination OFF.
Lines/Page:
Paginatio
12. Make the Title Alignment Left, clear the Title textbox and enter these four separate lines for the title:
Alignment: Left
TITLE
$NNODES$MAXNOD$DEFMAX$NDMAX$NWIDTH
SUBTITLE1
SUBTITLE2
Of course you can substitute anything you want for TITLE,
SUBTITLE1 and SUBTITLE2.
13. Turn OFF Display Column Labels.
Display Column Lab
Column
1
2
Column Lbl Value Format
Entity ID %I8%
X Component > %E13.7%
14. Now in the spreadsheet, click on the Value Format cell for
Entity ID. Change the format to %I8%. You do this by changing the data in the Input databox above the spreadsheet and pressing the Enter or Return key to accept the data.
15. For all other results quantities click on their respective
Value Format cells and change the formats to %E13.7%. (If you have more results quantities than will properly fit in 80 columns, then put a %E13.7%%1N% in any that extend beyond 80 columns to force it to start on a new line.) Press the OK button on this form.
OK
17. (Optional) Change to Target Entities. Select any specific target entities you may want in the report but more importantly for this example make sure that Entity
Attributes (Display Control) is set to Nodes.
Additional Display Con
Nodes
18. (Optional) Since this example requires a fair amount of setup it would be wise to save this report with a specific name if necessary to recall it later for making more .
nod
files.
Do this in Plot Options. Enter a name for the report like
nod_file.
Save Report As: nod_file
19. Press the Apply button.
Apply
TITLE
810 1468 -2.524668e-03 257 3
SUBTITLE1
SUBTITLE2
1 2.2122014E-4-2.1767017E-4 5.1733572E-3
2 2.3673585E-4-2.1802561E-4 5.1421551E-3
3 2.5836058E-4-2.1974165E-4 5.1010177E-3
4 2.8729768E-4-2.2396364E-4 5.0501702E-3
5 3.2454749E-4-2.3185805E-4 4.9901465E-3
6 1.9807677E-4-1.9593856E-4 5.1675760E-3
7 2.1360462E-4-1.9616591E-4 5.1363972E-3
8 2.3523276E-4-1.9754541E-4 5.0952709E-3
9 2.6418973E-4-2.0135389E-4 5.0444230E-3
10 3.0147523E-4-2.0885997E-4 4.9843905E-3
11 1.7493652E-4-1.7423423E-4 5.1618074E-3
12 1.9049116E-4-1.7429129E-4 5.1305941E-3
.
.
.
Figure 10-3 Example of a Formatted MSC.Patran .nod File.
CHAPTER 10
Reports
183
9
9
184
PART 6
Results Postprocessing
Create a MSC.Patran .els Formatted File.
A MSC.Patran .els file is an element based ASCII results file. The format of this file is:
Record 1:
Record 2:
Record 3:
Record 4:
TITLE
NWIDTH
SUBTITLE1
SUBTITLE2
Record 5 To N+4: ID, NSHAPE, (DATA(J), J=1,NWIDTH) (2I8, /, (6E13.7))
(80A1)
(I5)
(80A1)
(80A1) where:
TITLE
SUBTITLE1
SUBTITLE2
NWIDTH
ID
NSHAPE
DATA
80A1 Title Stored In An 80 Word Real Or Integer Array.
Same format as TITLE.
Same format as TITLE.
Number Of Columns Of Data Stored In The File (Integer).
Element Identification Number (Integer).
Essential Shape Code (Bar = 2, Tri = 3, Quad = 4, Tet = 5, Pyr = 6, Wedg = 7, Hex =
8; Integer).
Result Quantities Organized By Column Index (Real).
1. Set the Method to Overwrite File. By default, new file will be
Method: Overwrite File
created called patran.prt.1
. It will be changed later.
2. In Select Results mode. Select the Result Case from the first listbox.
3. Select a result from the second listbox.
4. (Optional) If necessary, select a layer. For this example, only one layer can be selected for a proper .
els
file to be created.
5. Select the Quantities to output to the file. Select NSHAPE as the first quantity and then any element based results you wish to output to the .
els
file. Only real (floating point data) quantities are valid for proper .
nod
files.
6. Go to Display Attributes.
Position...(at Z1)
7. Press the Format... button.
8. Change the file name to patran.els
.
9. Set the File Width to 80.
10. Clear the Lines/Page, Top Margin, and Left Margin databox or put zeros.
Format
File Width: 80
Lines/Page:
CHAPTER 10
Reports
185
11. Turn Pagination OFF.
Paginatio
12. Make the Title Alignment Left, clear the Title textbox and enter these four separate lines for the title:
TITLE
$NWIDTH
SUBTITLE1
SUBTITLE2
Of course you can substitute anything you want for TITLE,
SUBTITLE1 and SUBTITLE2.
Alignment: Left
13. Turn OFF Display Column Labels.
Display Column Lab
Column
1
2
Column Lbl Value Format
Entity ID %I8%
NSHAPE %I8%%1N%
14. Now in the spreadsheet, click on the Value Format cell for
Entity ID. Change the format to %I8%. You do this by changing the data in the Input databox above the spreadsheet and pressing the Enter or Return key to accept the data.
15. Change the Value Format for NSHAPE to %I8%%1N%.
16. For all other results quantities click on their respective
Value Format cells and change the formats to %E13.7%. (If you have more results quantities than will properly fit in 80 columns, then put a %E13.7%%1N% in any that extend beyond 80 columns to force it to start on a new line.) Press
OK when done.
OK
17. In Display Attributes also set the Report Type to Data Only.
Report Type:Data Only
18. (Optional) Change to Target Entities. Select any specific target entities you may want in the report but more importantly for this example make sure that Entity
Attributes (Display Control) is set to Element Centroids since only one value per element can be output to a proper
.
els
file.
Additional Display Con
Element Centroids
19. (Optional) Since this example requires a fair amount of setup it would be wise to save this report with a specific name if necessary to recall it later for making more .
els
files.
Do this in Plot Options. Enter a name for the report like
els_file.
Save Report As: els_file
20. Press the Apply button.
Apply
9
9
186
PART 6
Results Postprocessing
TITLE
6
SUBTITLE1
SUBTITLE2
1 4
-8.3064389E-1-9.9953584E-2 0.0000000E+0 1.6953596E-1 0.0000000E+0 0.0000000E+0
2 4
-7.7712482E-1 1.5068005E-1 0.0000000E+0 1.2687577E-1 0.0000000E+0 0.0000000E+0
3 4
-8.5500902E-1 9.5036231E-2 0.0000000E+0 1.5014736E-3 0.0000000E+0 0.0000000E+0
4 4
-5.8506662E-1-3.0595655E-2 0.0000000E+0 1.1098222E-2 0.0000000E+0 0.0000000E+0
5 4
1.7681476E-1 1.2351368E-1 0.0000000E+0 1.2829211E-1 0.0000000E+0 0.0000000E+0
.
.
.
Figure 10-4 Example of a Formatted MSC.Patran .els File.
CHAPTER 10
Reports
187
View Global Variables in a Report.
Global variables are generally single results values associated with an entire Result Case. For instance the load case number is a global variable.
Time, frequency, eigenvector, mode number, design variable and design cycle are also global variables. To view such global variables there are two methods.
1. Select a single Result Case and result quantities for a report as explained in previous examples.
2. Under Display Attributes, press the Format button and in the Title, Header, or Footer textbox include the variable
$GV:<name>, where <name> is the name of the global variable you wish to output. (If you are not sure what the available global variable names are you can always set the
Object to Graph, select a few Result Cases and then you can see a list of global variables in the option pull down at the bottom of the form with X or Y value set to Global Variable.)
3. Press the Apply button and your global variables will be reported in the Title, Header, or Footer of your report.
Or another way is to:
•
Select Result Cases and result quantities as explained previously.
•
Go to Plot Options and set the Report Type to
Summary.
•
Press the Apply button. Some global variables are reported in the summary table for each Result Case selected.
Format
Apply
Apply
MSC.Patran Version x.x 05/13/97 11:46:58 AM
Analysis Code: MSC.Nastran
Load Case: DEFAULT, Mode 9:Freq.=56.47 ;Eign=125890.898438
Result: Eigenvectors, Translational- Layer (NON-LAYERED)
Entity: Node Vector
SUMMARY INFORMATION
Maximum value - Node ID: 16, value: 0.001634
Minimum value - Node ID: 34, value: -0.009729
Figure 10-5 Global Variables Reported in Title for a Single Result Case
9
9
188
PART 6
Results Postprocessing
Reporting Element Nodal Data.
Some results are associated with nodes, others with elements.
When results are associated with elements yet you wish to see the contributions at each node due to that element, the report application will do so for you. This will also work if you wish to see the actual values at quadrature points (gauss points) inside the element.
1. Select Result Case and result quantities for a report as explained in previous examples but make sure the results are element based such as a stress tensor (displacement and constraint forces are nodal based).
2. Go to Target Entities and make sure that the target entities selected are to be displayed or reported at Element Nodes.
Additional Display Con
Element Nodes
3. Go to Display Attributes. Press the Format button. You will note that in the columns to be reported are the Node ID as well as the Entity ID. The entity ID will be the element number and the Node ID will be the node ID to which a particular row of results is associated for that element ID. If results are at gauss or quadrature points, the Node ID will be reported as Position ID instead which is an internal ID to
MSC.Patran. (Target entity display must be set at Element
All Data for Position IDs.)
4. Press the Apply button to generate the report.
Format
Apply
MSC.Patran Version x.x 05/13/97 11:46:58 AM
Analysis Code: MSC.Nastran
Load Case: DEFAULT, Mode 9:Freq.=56.47 ;Eign=125890.898438
Result: Eigenvectors, Translational- Layer (NON-LAYERED)
Entity: Node Vector
-Entity ID--X Component---Y Component---Z Component---Node ID-
1 4.469031E+5 1.474780E+5 0.000000E+0 1
1 4.172904E+5 3.858846E+4 0.000000E+0 2
1 1.171948E+5 -7.628262E+2 0.000000E+0 11
1 1.271206E+5 4.194981E+4 0.000000E+0 10
2 4.172904E+5 3.858846E+4 0.000000E+0 2
2 4.272350E+5 5.582101E+4 0.000000E+0 3
2 1.191011E+5 -7.161045E+2 0.000000E+0 12
2 1.171948E+5 -7.628262E+2 0.000000E+0 11
3 4.272350E+5 5.582101E+4 0.000000E+0 3
3 4.236081E+5 5.343995E+4 0.000000E+0 4
3 1.151038E+5 3.807227E+2 0.000000E+0 13
3 1.191011E+5 -7.161045E+2 0.000000E+0 12
.
.
.
Figure 10-6 Example of Element Nodal Based Report
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
11
Create Results
■
■
■
■
■
190
PART 6
Results Postprocessing
11.1
Overview
For an overview of how the Results Application works please see
(p. 1). Results can be derived, combined or created in a variety of ways.
Action:
Create
Object:
Results
Method:
Combine
New Result Case Name
Combine
New Subcase Name
Subcase 42
Select Result Cases
Load Case 1, Time=0
Load Case 1, Time=0.05
Create Results - to create results set the Method to the desired type. Results can be Combined and
Derived or fictitious results can be created for demonstration and testing purposes.
10
-Apply-
Combined Results:
This Method allows for the scaling and combining of selected Result Cases.
This is most commonly used for linear superposition of subcases. Although most analysis codes feature subcase superposition, this operation can also be done in MSC.Patran while the analysis code solves for only the individual subcases. Combining results using this method is limited to scaling each selected Result Case and then adding together the individually selected Results
Cases to create a new Result Case and subcase. Common results quantities must be selected for the combination and each Result Case must be associated with the same finite element entities.
A detailed explanation of this Method is described in
Derived Results:
This Method can be set to Maximum, Minimum, Sum, Average, and PCL
Function to allow for derivation of results quantities in a variety of different manners. New results may be derived from maximum/minimum values from selected Result Cases and/or layer positions or results may be used in a PCL expression to derive a new result quantity.
Derived results differ from combined results in two ways: (1) results to be derived may belong to different sets of nodes or elements which may or may not be disjointed whereas results to be combined must belong to exactly the same entities; and, (2) derived results are computed by varying procedures whereas combined results are computed by linear combinations (sum of scaled values). A detailed explanation of these Methods are described in
Demo Results:
This capability is more meant for simple creation of results for demonstration and testing purposes when no results are available. See
CHAPTER 11
Create Results
191
11.2
Combined Results
For performing combinations of Result Cases the form appears as shown below. This is the capability of linear superposition of subcases and/or for simple scaling of results. To combine results follow these general instructions:
Action:
Results Display
Create
Object:
Results
Method:
Combine
New Result Case Name
Combine
New Subcase Name subcase 5
Select Result Cases
Load Case 1, subcase 1
Load Case 1, subcase 2
Load Case 1, subcase 3
Load Case 1, subcase 4
Step 1:
Enter a name for the combined New Result
Case Name that will be created. This can be an existing Results Case Name.
Step 2:
Enter a New Subcase Name. If the New
Results Case name exists already, then the subcase will be added to the already existing subcases of that
Result Case.
Step 3:
Select the desired Result Cases from this listbox.
Each Result Case is selected individually. You cannot drag pick in this listbox to select multiple Result Cases. When you select one of these Result Cases a subordinate form will appear to allow specification of the scale factors. This is explained in more detail below.
Step 4:
Press the Apply button on the bottom of the form to create the new combined Results
Case.
-Apply-
10
192
PART 6
Results Postprocessing
When a Result Case is selected in the listbox a subordinate form appears. This is a simple form to specify the scale factors to be applied to each selected Result Case and for specifying which results associated with the Result Cases will be combined into the new Result Case, subcase.
Once the Apply button is pressed the new Result Case, subcase will be available to postprocess.
To change the scale factor of one of the Results Cases, first select the Factor cell and then type an new factor in the Input Scale Factor databox. Press the Enter key to acceptance the new scale factor.
Combine Result Cases
Input Scale Factor:
1.0
Combine Results Cases
Factor
Load Case 1, Subcase 1
Load Case 1, Subcase 2
Load Case 1, Subcase 3
1.0
1.0
1.0
Select Results
Bar Stresses, Compression Safety Margin
Bar Stresses, Maximum Axial
Bar Stresses, Minimum Axial
Displacements, Translational
Stress Tensor,
10
OK
Select the Result or Results associated with these Result Cases that you wish to retain in the new combined Result Case.
To add or remove Result Cases from this form simply select or deselect the Result Cases from the listbox on the main Results application form. As you do this, rows will be added or deleted from the spreadsheet on this form. Press the OK button when everything is set as desired. Press the Apply button on the main form to create the new results. If you need to change scale factors or the selected results to retain, select or deselect a Result Case and this form will reappear allowing for changes.
CHAPTER 11
Create Results
193
11.3
Derived Results
Deriving results is a powerful tool and gives a fair amount of flexibility. In this respect, Derived
Results differs from Combined Results significantly. If only a simple global scaling of a Result
Case is desired or the scaling and/or addition of one or more like Result Cases (subcases) is
desired, then it is advisable to use Combined Results as explained in
(p. 191). When more complex derivations are needed such as extracting the maximum or
minimum values from multiple layers and Result Cases or creating a new results quantity, then the derive capability must be used. Derive Results can be as simple as extracting max/min values or as complex as creating PCL expressions to derive new results. There are therefore, five
Methods available to derive results: Maximum, Minimum, Sum, Average, and PCL Function.
Derived results can only be created. There is no Modify function for derived results.
Toggles the form to select results for derivations when the Method is set to
Maximum, Minimum, Average, Sum, or PCL Function.
To derive results, these basic operations must be followed:
1. Set the Action to Create, the Object to Results and the Method to the function you wish to perform. Is it the extraction of max/min values, averaging or summing, or a more complicated expression that will have to be define with a PCL function? Set this with the Method pulldown at the top of the form.
2. Select a Result Case or Cases from the Select Result Case(s) listbox. See
(p. 15) for a detailed explanation of this process as well
as
3. Define a new name for the derived result. Default names can be accepted and no action is required.
4. Select a Result from the second listbox. It is important to understand that whatever result type is selected, the same result type will be created. That is if the result type is scalar, vector or tensor, then the newly derived result will be either a scalar, vector or tensor, respectively.
10
194
PART 6
Results Postprocessing
10
5. For Average, Sum, and PCL Function derivations skip to step
Otherwise select the Quantity for comparison purposes, such as von
Mises, from the Quantity option pulldown menu. The following quantities are available from vector and tensor data.
Vector to Scalar.
Magnitude, X Component, Y Component, Z
Component.
Tensor to Scalar.
von Mises, XX, YY, ZZ, XY, YZ, XZ, Minor,
Intermediate, Major, Hydrostatic, 1st Invariant, 2nd Invariant, 3rd
Invariant, Tresca, Max Shear, Octahedral. See
For vector or tensor result types a resolution to the selected scalar quantity is made for comparison purposes only. The resulting result remains a vector or tensor.
6. If more than one layer is associated with the selected result, select the layer(s) from which you wish to derive results using the Position button.
7. Skip this step unless a PCL Function derivation is requested. If the function is the derivation of results based on a PCL function, then determine what the type of the new derived result will be. That is, will it be a scalar value, a vector, or a tensor? Then define the PCL expression.
This is explained below in
8. Optionally you can select target entities from which to derive results if you wish to limit where the new results are calculated. By default all entities associated with the selected Result Cases will be targeted.
However you may limit it to only particular selected entities as explained
(p. 200). Target entities are specified by pressing the
second button toggle on the top of the form.
9. Optionally you can set comparison criteria (Algebraic or Absolute) and other optional result manipulations such as scaling and coordinate transformations. This is explained in
10. Press the Apply button when ready to create the derived result.
Apply
Max/Min.
Once the Apply button is pressed, the following internal operations occur:
1. Any operations under Plot Options are performed. This includes coordinate transformations, scale factors, etc.
2. The scalar Quantity is derived from vector or tensor data. For scalar results, this step is not necessary.
3. The maximum or minimum comparison is done for each target entity based on the derived scalar result Quantity for vector/tensor data or the scalar result itself for scalar data.
4. What is kept from the comparison is not the Quantity itself, but the scalar, vector, or tensor values based on the Quantity comparison for each entity. The new results are stored in the database in the same form as the originally selected results. That is, nodal data remains nodal, element centroidal data remains as element centroidal, and element nodal or element gauss data remain as is. A single new Result Case of maximum or minimum data is created from this operation.
CHAPTER 11
Create Results
195
Average/Sum.
Once the Apply button is pressed, the following internal operations occur:
1. Any operations under Plot Options are performed. This includes coordinate transformations, scale factors, etc.
2. The individual components of the selected result type are summed separately for all selected Result Cases and layers. For vector data, the X, Y, and Z components are summed separately. For tensor data, the XX, YY, ZZ, XY, YZ, and ZX components are summed separately.
3. For the Average method, the sum of each component is then divided by the number of occurrences. For example, if at a particular node six Result Cases contain results, the average will be computed by adding the six together and dividing by six. It is possible to have a different number of results existing at different target entities.
4. The new results are stored in the database in the same form as the originally selected results. That is, nodal data remains nodal, element centroidal data remains as element centroidal, and element nodal or element gauss data remain as is. A single new Result
Case of averaged or summed data is created by this operation.
PCL Expressions.
Once a PCL expression has been defined and the Apply button is pressed, the following internal operations occur:
1. Any operations under Plot Options are performed. This includes coordinate transformations, scale factors, etc.
2. The PCL expression is applied to all results in the selected Result Cases and/or layers.
3. The new results are stored in the database in the form as indicated by the New Result
Type setting. Note that nodal data remains nodal, element centroidal data remains as element centroidal, and element nodal or element gauss data remain as is. A new
Result Case is created for every selected Result Case and a new layer for every selected layer.
10
196
PART 6
Results Postprocessing
The PCL Expression builder form is shown below. You may type in your own PCL equation but for most operations, the PCL expression can be built simply by pressing the arithmetic operator buttons and selecting intrinsic functions and/or independent variables from the listboxes. No typing is required unless you need to reference user defined PCL functions. For detailed information on how to write your own PCL functions see
Understanding PCL
(p. 2) in the PCL
and Customization.
Define PCL Expression
PCL Expression
$VONM + ABS( $ZX ) )
Type the PCL
Expression into this databox here or select listboxes and operators below.
Independent Variables
VONM
XX
YY
ZZ
XY
YZ
ZX
MAJOR
INTER
MINOR
HYDRO
INV1
Arithmetic Operators
+ * / **
Intrinsic Functions
ABS
ACOSD
ACOSR
ASIND
ASINR
ATAN2D
ATAN2R
( )
Use these buttons to help you build the arithmetic equations you need to define the expression.
Simply press one of them and the
Arithmetic Operator is placed in your equation.
OK
10
Depending on the Derived Scalar Type, various Independent Variables will be available to you for use in the PCL expression.
Works in the same fashion as the Arithmetic
Operators. Click on one and it will be placed in your equation. You must then place something as its argument such as one of the independent variables to the left.
The variables used in the PCL expression must begin with the $ sign, (i.e., $SCALAR). The variable simply signifies that when the expression is evaluated for a particular entity (say at a node), the results value for that entity will be used in the variable to derive the new result and this will be the case for every entity selected for the derivation.
Vectors require three function definitions. Tensors require six. These function definitions are separated by semi-colons (example: $XX; $YY; $ZZ/2).
The Independent Variables available for use in the PCL equation are dependent on what results type you have asked to derive. For derivations from scalar values, the only variable available is
$SCALAR. However when vector results have been selected you have the choice of these variables:
Vector to Scalar: $MAG (magnitude), $XX (X component), $YY (Y-component.), $ZZ
(Z-component.). See
CHAPTER 11
Create Results
197
For tensor results you have the choices of these variables:
Tensor to Scalar: $VONM (von Mises), $XX, $YY, $ZZ, $XY, $YZ, $ZX, $MINOR,
$INTER, $MAJOR, $HYDRO, $INV1, $INV2, $INV3, $TRESCA, $MAXSHR, $OCT. See
The intrinsic functions available for scalar derived results are:
Function
ABS(value)
ACOSD(value)
ACOSR(value)
ASIND(value)
ASINR(value)
ATAND(value)
ATANR(value)
ATAN2D(x, y)
ATAN2R(x, y)
COSD(angle)
COSR(angle)
EXP(value)
LN(value)
LOG(value)
SIND(angle)
SINR(angle)
SQRT(value)
TAND(angle)
Description
Returns the absolute value of the result argument.
Returns the angle in degrees which corresponds to the trigonometric cosine of the result contained in the argument.
Returns the angle in radians which corresponds to the trigonometric cosine of the result contained in the argument.
Returns the angle in degrees which corresponds to the trigonometric sine of the result contained in the argument.
Returns the angle in radians which corresponds to the trigonometric sine of the result contained in the argument.
Returns the angle in degrees which corresponds to the trigonometric tangent of the result contained in the argument.
Returns the angle in radians which corresponds to the trigonometric tangent of the result contained in the argument.
Returns the angle in degrees to the trigonometric tangent represented by the specified x and y components in the argument.
Returns the angle in radians which corresponds to the trigonometric cosine of the result contained in the argument.
Returns the trigonometric cosine value of the result argument specified in degrees.
Returns the trigonometric cosine value of the result argument specified in radians.
Returns the power function of natural logarithm base, e to the x, where x is the result value argument.
Returns the natural logarithm of the result argument.
Returns the common logarithm (base 10) of the result argument.
Returns the trigonometric sine value of the result argument specified in degrees.
Returns the trigonometric sine value of the result argument specified in radians.
Returns the square root of the result argument.
Returns the trigonometric tangent value of the result argument specified in degrees.
10
198
PART 6
Results Postprocessing
Function
TANR(angle)
User Defined
Description
Returns the trigonometric tangent value of the result argument specified in radians.
Any user defined function that can accept a scalar, vector, or tensor array may be used. For example you might have function defined in
MSC.Patran called my_result_function. You would then type it in manually and enter one, or more of the independent variables separated by commas, i.e., my_result_function($XX, $YY, $ZZ). Inside your function $XX, $YY, and $ZZ are defined as REAL variables. For vector and tensors, the function parameters must be defined as REAL 3x1 and
3x3 dimensioned variables respectively. The return value must be the same as the type of new result being created: scalar, vector, or tensor. See
All intrinsic function accept a single scalar quantities as input, e.g., SIND($XX) except ATAN2D and ATAN2R. Also note that PCL derived results from as-is coordinate systems results in a new result in an undefined coordinate system. The new result can there for not be transformed into any other coordinate system. To avoid this it is suggested to derive the new results in a know, consistent coordinate system such as the Global system.
Examples:
Function
LN($SCALAR)
$XX;$YY;$ZZ
$XX+$YY;$YY+$ZZ;0.0
$ZX;$YZ;$XY;$ZZ;$YY;$XX
Description
Would generate the natural log of the variable $SCALAR when deriving a new scalar result.
Would generate a vector replicating the input result.
Would generate some sort of user modified result with the
Z component of the vector set to 0.0.
Would swap the order of the components in a tensor.
10
CHAPTER 11
Create Results
199
User Defined PCL.
You may enter your own user defined PCL functions also that have been compiled into MSC.Patran. A user defined PCL function must be set up to accept scalar values as the parameters and return a single scalar value. Any number of scalar parameter inputs may be defined. For example you may enter a function:
myFunction( $XX, $YY, $ZZ )
The contents of your PCL functions might look something like:
FUNCTION myFunction( x, y, z )
REAL x, y, z /* these are real scalars */
RETURN x+y+z
END FUNCTION
/* must return a scalar value */
To use this function, enter it as you would a variable (no $ sign however). Examples:
Function Description
LN(myFunction($XX, $YY, $ZZ))
Would generate the natural log of the returning value form myFunction when deriving a new scalar result.
myFunction($XX, $YY, $ZZ);2.0;2.0
Would generate a vector with the returning value of myFunction as the first component and the second and third set to 2.0.
For more information on how to create and compile PCL functions see
The PATRAN Command
Language (PCL) Introduction
(Ch. 2) in the PCL and Customization.
10
200
PART 6
Results Postprocessing
10
Target Entities
Similar to the other graphical plot tools in the Results application, derived results can be limited to various entities via the Target Entities options.
Toggles the form to select target entities for creating derived results.
You may wish to derive results for only a few elements or nodes or those entities associated with a group or group of groups.
The following table describes in detail to which entities derived results can be targeted:
Entity Description
Entire Model
Current Viewport
The derived results can be limited to only the entities (nodes or elements) associated with everything in the currently active viewport.
Nodes
Individual nodes may be selected from which to create a graph. Nodes are selected graphically from the screen and fill the databox. However, you may type in any node numbers manually. Be sure to include the word Node in front of the IDs you type in manually, (i.e., Node 1 5 55
100 etc.). Elemental based results are extrapolated to the nodes and averaged.
Elements
This is the default option where derivations will be performed for all entities (nodes or elements) associated with the selected results. No consideration or selection of any graphical entities is necessary.
Individual elements may be selected for which to derive results.
Elements are selected graphically from the screen and fill the databox.
However, you may type in any element numbers manually or by selecting them graphically from the screen. Be sure to include the word
Elem in front of the IDs you type in manually, (i.e., Elem 1 5 55 100 etc.).
With elemental data, values will be extrapolated or averaged to the element centroid for reporting purposes.
Groups
Materials
Properties
Element Types
Derived results can be limited to only selected groups. A selected group or groups must have nodes or elements in them otherwise the derivation will not work. A listbox allows selection of the group(s) for which the derived results will be calculated.
Derived results can be targeted at only those finite elements which have certain material properties assigned to them. A listbox appears allowing selection of the materials for whose elements will be targeted.
Derived results can be targeted at only those finite elements which have certain element properties assigned to them. A listbox appears allowing selection of the properties for whose elements will be targeted for a fringe display.
Derived results can be limited to only certain element types also.
Important:
Once a target entity has been selected, it will remain the target entity for derived results until the user physically changes it.
CHAPTER 11
Create Results
201
Result Options
Derived results have various options that are available for specifying how and what operations are to be performed.
Result Options selection button. Toggles the form to select Results options for derived results.
The following table describes in detail the Derived results options which can be modified:
Option
Coordinate
Transformations
Scale Factor
Comparison
Criteria
Save Derived
Results
Description
Vector and tensor results can be transformed into any of the following coordinate systems: any user defined local system (CID), the projection of any CID, the MSC.Patran global system, a material coordinate system, element IJK coordinate system or the nodal
(analysis) coordinate system depending on the type of result (vector, or tensor). See
(p. 305) for a definition of each
of these coordinate systems. The default is no transformation, which will derive data in the coordinate frame as stored in the database.
Typically the solver code will calculate results at nodes in the analysis coordinate system specified by the user. These can vary from node to node. Element data can be stored from the analysis code in any coordinate system.
This scale factor has the effect of simply scaling the results up or down by the specified amount before derivation.
When doing maximum or minumum comparisons this toggle indicates the type of comparison to be made. Algebraic will consider the sign, negative numbers being less than positive numbers.
Absolute will ingnore the sign and compare only the relative magnitude. Example: Comparing -6 to 5 algebraically will render 5 larger than -6, yet absolutely, -6 is larger than 5.
If this toggle is OFF, then no new Result Case and/or subcase will be created. The new result will simply be stored in a results register.
This is not too terribly useful unless you are doing PCL programming and understand the use of registers.
10
Important:
Once plot options have been selected, they will remain in effect for the derivation until the user physically changes them.
202
PART 6
Results Postprocessing
11.4
Demo Results
This form appears when the Method is set to Demo when creating results. This form allows the creation of results for demonstration and testing purposes. Demo results can be either nodal or element results. Scalar, vector and tensor result types can be created, and scale factors may be applied.
Results Display
Action:
Create
Object:
Results
Method:
Demo
Existing Result Cases
Load Case 1, Time=0.
Load Case 1, Time=0.05
Load Case 1, Time=0.1
To create Demo results on models that have no results associated with them for testing or demonstration purposes set the Method to Demo.
Result Case Name
Derived Results, Demo
Select an existing Results Case in which to place the Demo results or type in a new name in the databox. You must supply a Results Case and a Subcase separated by a comma and a space.
Result Location
Nodal Element
Scale Factor
1.0
Create either nodal based or element based results and supply a scale factor if desired. If elemental based results are selected, you must also identify where to create the results
(Centroid, Nodes, Gauss points, etc.)
10
Result Data Type
Scalar Vector Tensor
Result Generation Method
Sine Function Unit Load
Nodal Data System:
Global
-Apply-
Identify what type of data to be created (Scalar, Vector,
Tensor).
Two methods are available to create demo results:
1. By product of f(x) * g(y) * h(z) where f(x), g(y) and h(z) are sine and cosine functions on the bounding box that encloses the model. The choice of functions depends on the remainder of the scale factor divided by (i.e., factor modulo 8).
Results are also scaled by this factor. This method should be used if greatly varying results in the model are desired.
2. By unit load applied to the corner of the bounding box that encloses the model. The bounding box is extended to prevent singularity at the application point. The location of the unit load depends on the value of factor modulo 8. Results are also scaled by this factor. This method should be used if gradually varying results in the model are desired.
Identify the coordinate system in which to associate the results. Press the Apply button to create the results.
CHAPTER 11
Create Results
203
11.5
Examples of Usage
The following are a few typical usages of the Create/Results option in the Results application.
In particular are simple examples of results combination and derivations. The examples assume the Action is set to Create and the Object set to Results.
Perform Linear Subcase Superposition
This example assumes you have two linear static analysis load cases, X and Y, and you wish to combine them to create subcase Z = X + 2Y.
1. Set the Method to Combine.
Method:
Combine
2. Supply a new Result Case name if desired or accept the default. If you wish the new result to be a new subcase of an existing set of Result Cases then type in the same primary name as the results that you will select for combining.
3. Enter a new Subcase name (Z) or accept the default.
New Result Case Name:
Combine
New Subcase Name:
Xplus2Y
4. Select from the listbox the Result Cases (X and Y) that you want to combine. When you select one, a subordinate form will appear allowing you to set scale factors and select the results to retain in the new combined result.
Continue to select all the Result Cases you wish to combine. They will all appear in the other form. If you make a mistake simply deselect the Result Case.
5. If you wish to scale any one of the Result Cases, click on the cell which contains the Factor you wish to change on the subordinate form. In the databox at the top of the form type in a new scale factor and press the Return or Enter key to accept it. For the Y subcase this factor is changed to
2.0.
Input Scale Factor:
2.0
6. From the Combine Result Cases form also select the results you wish to retain in the new combined result.
You may close this form down now if desired by pressing the OK button.
7. Press the Apply button.
OK
Apply
10
204
PART 6
Results Postprocessing
+
Y
X
=
Y
X
10
Y
X
Figure 11-1 Linear Superposition of Two Load Cases to Create a Third
Derive the Maximum von Mises Stress from Multiple Layers and Subcases
This example assumes you have multiple Result Cases and that there are layers of results (such as top and bottom surface stresses) associated with each. The goal is to produce one result of the maximum von Mises stress from any given load case and layer.
1. Set the Method to Maximum.
Method:
Maximum
2. Select all the Result Cases of interest from which you want to extract the maximum values from in the top listbox.
3. Enter a new name for the derived result if desired or accept the default.
New Result Case Name:
Derived Results
4. Enter a new Subcase name or accept the default.
New Subcase Name:
MaxvonMises
5. Select either a stress tensor result or a scalar von Mises result from the second listbox.
6. If you selected a stress tensor, also change the result
Quantity to von Mises.
Quantity: von Mises
CHAPTER 11
Create Results
205
7. Select all the layers from which you want to extract the maximum values using the Positions button. The ellipses after the position name indicate that more than one layer is selected.
8. (Optional) Change the mode of Results Application to the
Result Options form (press the right most button icon).
Make any option changes necessary.
9. Press the Apply button.
Position...(at Point C...)
Apply
Layer1
Y
X
Layer2
Y
X
Maximum
Y
X
Figure 11-2 Maximum Plot of Two Different Layers
10
206
PART 6
Results Postprocessing
Derive von Mises Stresses in Neutral Ply Using Average Method
This example assumes you have shell elements with two layers, top and bottom. The goal is to produce one result of the average von Mises stress from the top and bottom layer, or in other word, find the von Mises stress at the neutral ply.
1. Set the Method to Average.
Method:
Average
2. Select all the Result Case of interest from the top listbox.
10
3. Enter a new name for the derived result if desired or accept the default.
New Result Case Name:
Derived Results
4. Enter a new Subcase name or accept the default.
New Subcase Name:
Ave_vonMises
5. Select Stress Tensor result from the second listbox.
6. Select all the layers from which you want to average using the Positions button (Z1 and Z2). The ellipses after the position name indicate that more than one layer is selected.
7. (Optional) Change the mode of Results Application to the
Result Options form (press the right most button icon).
Make any option changes necessary.
8. Press the Apply button.
Position...(at Point Z1..)
Apply
9. Go to Create/Fringe and select the new Result Case and the
Action:
new result and plot von Mises stress.
von Mises stress was not actually calculated or derived until
Object:
the fringe plot was made. The averaging was done over the components of the tensor only and the derived results were stored as a tensor. von Mises stress was derived from the tensor when the fringe plot was made. This mode of averaging is different than the Averaging technique available from the option pulldown menu in the Positions form where the actual von Mises stresses would have been calculated and then averaged as opposed to averaging the stress tensor components first. These two methods of averaging can result in vastly different numbers being reported. See
. The average von Mises stresses at the neutral ply in pure bending should be close to zero with the component based averaging as done in this example. The scalar based averaging will produce almost the same von Mises stress as seen in the top or bottom layers.
Create
Fringe
CHAPTER 11
Create Results
207
Top Layer- Z1
Y
X
Y
X
Y
X
Y
X
Bottom Layer - Z2 Component
Scalar
Based
Based
Averaging
Averaging from Create/Results from Positions Form
Figure 11-3 Average Plots of Two Different Layers.
To Create a New Result from the Components of a Tensor Using PCL
This example takes the X component of a stress tensor and multiplies it by the Y component and adds the Z component to the quantity.
1. Set the Method to PCL Function.
Method:PCL Function
2. Select all the Result Case of interest from which you want to derive new results in the top listbox.
3. Enter a new name for the derived results or accept the defaults.
New Result Case Name:
Derived Results
4. Enter a new Subcase name or accept the default.
New Subcase Name:
XtimesYplusZ
5. Select the result of interest from the second listbox, in this case a tensor quantity.
6. Change the New Result Type to Scalar.
New Result Type: Scalar
7. (Optional) Select a layers from which you want to derive results if necessary.
8. Press the Define PCL Expression button. A subordinate form will appear. You will create an equation that looks like
$XX * $YY + $ZZ. You can either type this into the textbox at the top of the form or you can create it by selecting the appropriate variables and operators in the order necessary to create the equation.
9. (Optional) Change the mode of Results Application to the
Result Options form (press the right most button icon).
Change any result option that are necessary.
10. Press the Apply button.
Position...(at Z1..)
Define PCL Expression
Apply
10
208
PART 6
Results Postprocessing
10
To Create a New Result with User Defined PCL
This example is identical to the previous example except it does it with a User Defined PCL function.
1. First define a PCL function in an external file called myFunction.pcl
as:
FUNCTION myFunction( x, y, z )
REAL x, y, z
RETURN x*y+z
END FUNCTION
2. Start MSC.Patran and issue the command:
!!INPUT myFunction
3. Set the Method to PCL Function.
Method:
PCL Function
4. Select all the Result Cases of interest from which you want to derive new results in the top listbox.
5. Enter a new name for the derived results or accept the defaults.
New Result Case Name:
Derived Results
6. Enter a new Subcase name or accept the default.
New Subcase Name:
XtimesYplusZ
7. Select the result of interest from the second listbox, in this case a tensor quantity.
8. Change the New Result Type to Scalar.
New Result Type:Scalar
9. (Optional) Select a layers from which you want to derive results if necessary.
10. Press the Define PCL Expression button. A subordinate form will appear. This time you will enter your PCL function as:
myFunction( $XX , $YY , $ZZ )
You must type this into the textbox at the top of the form, however you can enter the variables by selecting the appropriate ones from the Independent Variables listbox.
11. (Optional) Change the mode of Results Application to the
Result Options form (press the right most button icon).
Change any result option that are necessary.
12. Press the Apply button.
Position...(at Z1..)
Define PCL Expression
Apply
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
12
Freebody Plots
■
■
■
■
■
Create Loads or Boundary Conditions
■
■
210
PART 6
Results Postprocessing
12.1
Overview
This application allows for quick and easy graphical display of freebody diagrams. Also the individual components that make up a freebody diagram can be plotted independently such as reaction forces, applied loads and internal/external loads. This application is extremely useful for graphical display of these quantities, checking for equilibrium and creating loading or boundary conditions. Once a plot is displayed, it can be converted into an equivalent load or boundary condition set for subsequent use in another analysis.
For an overview of how the Results Application works please see
(p. 1). To specifically make freebody plot, select Create from the Action pull-
down menu on the Results application form; and select Freebody from the Object pull-down menu. The requirements and options available for a freebody plot are different than other plot types in the Results application. It is suggested that you fully read this overview and subsequent section carefully to understand how freebody plots are created in MSC.Patran.
11
This feature has been tailored specifically after data available from the Grid Point Force Balance
Table produced from a MSC.Nastran analysis with the case control request GPFORCE = ALL.
Once the results data has been loaded into the MSC.Patran database, they are treated generically.
However, only MSC.Nastran results are currently supported for this feature as far as results import is concerned.
To create a freebody plot the following basic steps must be followed:
1. Set the Action to Create and the Object to Freebody.
2. Decide whether the plot will be a true freebody plot, a interface load, or forced displacement. Set the Method accordingly.
3. Select a Result Case or Cases from the Select Result Case(s) listbox.
See
(p. 216) for a detailed explanation of this
process.
4. For freebody and interface load plots select a Result Type from the second listbox.
5. Optionally change the summation point and transformation options if necessary.
CHAPTER 12
Freebody Plots
211
6. Select target entities. That is, define the freebody by selecting a portion of the model. More detail on this operation can be found in
7. If necessary, change any display attributes of the freebody vector plots. See
8. Press the Apply button when ready to create the freebody, interface, or displacement plot.
9. Open the tabular display for freebody load information if necessary for checking force and moment summation and equilibrium.
10. Finally if you wish to create a load or boundary condition from the
resulting plot, do so with the Save Data option. See
Create Loads or Boundary Conditions
Apply
Important:
The behavior of this plot type is somewhat different than other plots in that it cannot be saved or recalled (posted) at will. It is meant for interactive use within this Freebody application only. Once you leave this application, the freebody plots will be cleared from the screen.
11
212
PART 6
Results Postprocessing
Requirements.
The following form is a general appearance of the Freebody plot form with a brief description. There are certain requirements that must be met in order for any results to be present in the listboxes on this form.
Action:
Object:
Method:
Results Display
Create
Freebody
Loads
The Method can be Freebody Loads, Interface Loads, or Forced
Displacements.
Select Result Case
Load Case 1 (1 subcases)
Load Case 2 (1 subcases)
Load Case 3 (2 subcases)
Load Case 4 (5 subcases)
These icons change the display of the form to present different options for each Type. The first icon (default) displays the form as shown for
(p. 216). The second is for selecting
finite element
(p. 218). The third allows for
(p. 223) and the fifth brings up
a spread sheet for
Select Subcase
Static Subcase -- (2.2)
Static Subcase -- (2.4)
Displays any Result Cases that have Grid Point Force data associated with them. If listbox is empty, either no results exist in the database, or no grid point force data exists in the Result
Case(s). If more than one subcase is associated with a Result
Case, then another listbox will appear below this one to allow selection of the desired subcases to process.
11
Select Result Type
Freebody Loads
Applied Loads
Reaction Loads
Internal Loads
Other Loads
Summation Point
[0 0 0]
Transform Results
Select Coordinate Frame
Coord 0
Reset Plot
-Apply-
Defaults
The different result types can be Freebody, Applied, Reaction,
External, Internal, or Other loads. Pressing Apply will display the loads, in vector form, on the model currently displayed. This listbox is not presented when the Method is forced
Displacements.
Moments and Forces are summed about a specific point. By default this point is the origin, however it can be set to any geometric point, node or screen location using the select mechanism. Results can also be transformed to any other coordinate frame.
Pressing the Apply button will display the plot in the current viewport. The other two buttons will reset (erase) the plot and restore the default setting of the current display of the form.
CHAPTER 12
Freebody Plots
213
1. The MSC.Nastran analysis must be run with a GPFORCE=ALL entry in the case control called out for all subcases. (Also PARAM,POST,-1 must appear in the case control or bulk data section of the input file to ensure that the Grid Point Force Balance Table
(GPFB) is written to an OUTPUT2 file. This is taken care of automatically when
MSC.Patran is used to create the input deck.)
2. The results in the OUTPUT2 file must be loaded into the MSC.Patran database. Results are generally in the analysis coordinate system of the nodes as specified in the
MSC.Nastran input deck, however they will be converted to the basic coordinate system when used in this application.
3. Eight (8) separate vector results are loaded into the database from the GPFB table. The labels of these results can be seen in the general Results application when the Object is set to anything other than Freebody. They must not be altered or deleted or the
Freebody Results application will not recognize them and therefore will not display them. In certain cases, not all these results will be present. They will be treated as zero quantities in subsequent freebody calculations if certain results do not exist such as when no applied loads actually exist. The labels are:
Grid Point Forces, Elements
Grid Point Forces, Applied Loads
Grid Point Forces, Constraint Forces
Grid Point Forces, Total
Grid Point Moments, Elements
Grid Point Moments, Applied Loads
Grid Point Moments, Constraint Forces
Grid Point Moments, Total
Description of Grid Point Force Balance (GPFB) Results.
All of these base results above are vector data associated with nodes, except for the “Grid Point Forces/Moments, Elements” which are associated with elements. All of these results are accessible from other plot types in the
Results application as well as for Freebody however Freebody plots will process the results differently in order to give a true freebody diagram, calculate equilibrium by summing forces and moments, and allow creation of new loading and boundary conditions.
•
Grid Point Forces/Moments, Elements
- These results are vector data associated with elements. Each element position corresponds to a node of the element where the results value at that node is that element’s contribution to the total internal load for that particular node. Processing these data with the general plot tools in the Results application is somewhat meaningless.
•
Grid Point Forces/Moments, Applied Loads
- These are the nodal equivalenced applied loads of the model. They are vector data stored at the nodes. Processing these data with this application or the general plot tools in the Results application should be very similar.
•
Grid Point Forces/Moments, Constraint Forces
- These are the nodal equivalenced constraint forces at the restrained locations of the model. They are vector data stored at the nodes. Processing these data with this application or the general plot tools in the
Results application should be very similar.
11
214
PART 6
Results Postprocessing
11
•
Grid Point Forces/Moments, Total
- These are the total nodal equivalenced loads at each node of the model. They are vector data stored at the nodes. Normally they should all be zero when equilibrium exists. However, there are occasions when these values are not zero. This typically happens when multipoint constraints and rigid elements exist in the model since they are not taken into account in MSC.Nastran Grid Point
Force Balance Table.
Description of Freebody Tool Plots.
From the four types of GPFB results for both forces and moments, the Freebody Results application can evaluate and display six (6) different types of vector plots when the Method is set to freebody Loads or Interface loads plus displacement plots:
Freebody Loads
This is by far the most interesting and important vector display. It consists of determining the total internal loads for all externally exposed nodes on the model (these are determined by selecting target finite elements or by using what is displayed on the screen) and displaying them along with any applied and reaction loads. For equilibrium to exist all of these vector loads should add up to zero in each component direction. Occasionally this is not the case since MPC and rigid element contributions are not taken into account. This can be checked visually or via the freebody load spreadsheet available by picking the right most button icon on the parent form where a force and moment summation is presented.
Applied Loads
By selecting this result type, the nodal equivalenced applied loads of the model will be plotted in vector form on the displayed model. Similar operations can be done with Marker (Vector) plots with these data.
Reaction Loads
By selecting this result type, the nodal equivalenced reaction loads of the model will be plotted in vector form on the displayed model. Similar operations can be done with Marker (Vector) plots with these data.
Internal Loads
By selecting this result type, the nodal equivalenced total internal loads of the model will be plotted in vector form on the exposed nodes of the displayed model. The model can be cut up and different target finite elements may be selected to view the internal loads anywhere in the model.
External Loads
By selecting this result type, the nodal equivalenced total of all loads associated with those elements attached to the freebody (but not part of the freebody) along the boundary will be plotted in vector form.
Other Loads
The total loads (Applied + Reaction + Internal) will not sum to zero if rigid elements, MPCs, thermal loads, or other external influences not accounted for are present. By selecting this result type, these external influences are displayed.
Displacements
For forced displacements, the results are plotted as vector displacement data only on the external nodes of the freebody.
All vector values from all of the above results types are also reported tabularly to a spreadsheet including the summation of forces and moments to calculate totals and check equilibrium.
Three types of graphical display are possible each available as a Method of the Freebody application.
CHAPTER 12
Freebody Plots
215
•
Freebody Loads -
This type will allow for graphical vector display of freebody loads at all external (exposed) nodes of the target entities (elements) selected - that is, a freebody diagram. In order for this type to be graphically displayed, a freebody should be defined as a group of elements called the target entities. If no target entities are specified, the target entities will default to all displayed elements in the current viewport. In addition, each individual nodal equivalenced load type (applied, reaction, internal, external, other) that make up a freebody diagram can also be plotted in vector form on the exposed nodes of the displayed freebody. The model can be cut up and different target elements may be selected to view these anywhere in the model.
Moments and Forces will be summed about the specified Summation Point and will be transformed to another coordinate system if requested. By default all graphical displays are presented in the Global coordinate system unless a transformation is requested, even if the results are stored in the database in their analysis coordinate systems. If a new load condition is created from this, it will consist of a new force and/or moment field which will be referenced by the force and/or moment load.
•
Interface Loads -
This type allows for the calculation of the total forces and moments acting across a boundary. Graphically this displays a single vector quantity at the summation point due to the loads from selected nodes in the freebody. Target entities in this case are the elements making up the freebody and the nodes in the freebody that are to be used in calculating the interface load. Both must be selected. There is no default and an error will be issued if no target entities are selected. For example, you may wish to know the total equivalent force and moment at a location across a boundary interface (such as where a wing intersects a fuselage). Therefore you would select the node or location at which to sum the forces and moments (the Summation
Point) and then select the nodes along the interface and the elements to which those nodes belong as the target entities. Generally the summation point will also belong to the target entities but this is not a requirement. Results belonging to nodes not associated to the target elements will be ignored in the calculations. The reason for selecting nodes and elements is that the nodal forces and moments are used at the selected nodes and the internal elemental forces and moments from the selected elements. If a new load condition is created from this, it will consist of a new force and/or moment load at the node (summation point). If the location is something other than a node, you will be prompted if you would like to create a node at that location.
•
Forced Displacements -
This type of freebody plot simply displays displacement results at the external edges of the freebody in the form of vector quantities. The vectors are shown along the edges of the selected elements when the display attribute for displaying on free edges only is turned ON. The displacements can be saved as an enforced displacement boundary condition and then subsequently used in a local analysis of the freebody which will reproduce the exact displacement conditions.
11
216
PART 6
Results Postprocessing
11
12.2
Select Results
This is the default display of the Freebody plot form when it first appears to Select Results.
Toggles the form to select results for freebody plots. This is the default mode of the Freebody form.
The following table describes each widget entity in the freebody Select Results mode of the form:
Entity Description
Select Result Case
Select a Result Case from this listbox. If nothing appears in this listbox, be sure that the results have been imported and that Grid
Point Force results exist as described in the previous section. See
(p. 212). The number of subcases for the displayed
Results Cases is displayed to the right of the title. Multiple Result
Cases may be selected, but be aware that the display will cycle through them one at a time. Selecting multiple Result Cases makes the most sense when creating multiple loading conditions or automatic multiple hardcopy plots.
Select Subcase
If more than one subcase is associated with a Result Case, then another listbox will appear below this one to allow selection of the desired subcases to process. Again multiple subcases can be selected.
The behavior of selecting multiple subcases is multiple plot displays.
Select Result Type
The different result types can be Freebody, Applied, Reaction,
External, Internal, or Other loads. Pressing Apply will display the loads, in vector form, on the model currently displayed. This listbox is not presented when the Method is forced Displacements. An explanation of each of these plot types can be found in
Summation Point
Moments and Forces are summed about a specific point. By default this point is the origin, however it can be set to any geometric point, node or screen location using the select mechanism.
Transform Results
Results can also be transformed to any other defined coordinate frame. Turn this toggle ON if you wish to do a coordinate transformation.
Select Coordinate
Frame
When the Transform Results toggle has been turned ON, this widget will appear. Simply select the coordinate system graphically from the screen or type in the name of an existing coordinate frame such as
“Coord 1.”
Reset Plot
Defaults
This will remove any freebody plot from the graphics screen.
This will reset all widgets to their default values and will remove any plot.
CHAPTER 12
Freebody Plots
217
Press Apply at any time to create the desired vector plot. If no target entities have been selected, the default display is what is currently displayed on the screen except for Interface Loads which must have target entities selected. See
(p. 218). Any display attributes and target
entities previously set are retained when the Apply button is pressed. Reset Plot will erase all vector displays from the screen and Defaults will set the form back to its default settings.
Important:
Once a results are selected and any other settings set, they will remain until the user physically changes them, the Default or Reset buttons are pressed or the
Action/Object/Method is changed. This will clear the plot and set the settings to defaults.
11
218
PART 6
Results Postprocessing
11
12.3
Target Entities
This is the Target Entity display of the Freebody plot form. This form is used to define the actual freebody of the model. For Freebody Loads the default is to plot on the entire existing display.
Toggles the form to select target display entities for freebody plots.
This form creates a list of elements and/or nodes for defining the freebody for the freebody diagram or other vector display. The following table describes the widgets on this form and how to properly select target entities:
Entity
Select By
Auto Add/Remove
Select/Entities
Add/Remove
Undo
Description
Elements and nodes may be selected individually or by association to groups, material and element properties or adjacent elements. Set this pulldown to indicate which type of entity is to be selected. For freebody plots only elements are involved. For Interface Load plots both elements and nodes need to be selected which causes this to be a two step process. First select the nodes and then select the elements on one side or the other which will contribute to the determination of the interface load. For Forced Displacement plots, only elements are necessary to define except when bar elements are involved. Then it is necessary to define the outer edge with node picks since the selecting algorithm uses free edges as its criteria. Bar elements do not have free edges. The Adjacent Elements pick is convenient for adding layers or subtracting layers of elements.
If this toggle is set to either Auto Add or Auto Remove then whenever you graphically select an entity or pick from a listbox, all entities are automatically added or removed from the listbox that displays the freebody entities on this form.
This is the listbox that will display the freebody definition. This definition will be made up of a list of entities (nodes and/or elements). The textbox can be edited manually but this is not recommended in case the syntax is not followed properly. It is best to fill the textbox by graphically selecting entities or selecting entities from a listbox of groups, materials, or properties. If nothing is in this listbox when Apply is pressed, the Freebody Load plot will be applied to whatever is visible in the current display. The Interface
Loads require that you pick both target nodes and entities (see
Description of Freebody Tool Plots
Forced Displacements requires only elements except for bar elements which require nodes.
Press the Add or Remove buttons to add entities into the freebody entities listbox. You only need to do this if you have not turned on either Auto Add or Auto Remove or that option is not available to you. (You cannot remove adjacent bar elements).
Undo clears out the last operation done and reverts to previous selected entities. Multiple undoes are possible.
CHAPTER 12
Freebody Plots
219
Clear
Show Selected
Elements
Show All Posted
FEM
Entity
Create New Group
Include Nodes
Overwrite
Group Name
Create Group of
Entities
Reset Plot
Defaults
Description
Clear will clean out the Freebody Entities listbox completely and two
Clears will clear the Undo memory dimming the Undo button.
When switched ON, the viewport displays only what is in the
Freebody Entities listbox. The freebody or other vector plot can be displayed on the freebody with only the freebody displayed or with the entire posted model displayed.
If ON, the entire posted model will be displayed. The freebody or other vector plot can be displayed on the freebody with only the freebody displayed or with the entire posted model displayed.
Turn this toggle ON if you wish to create a group from the selected target entities that define the freebody.
If this toggle is ON the nodes of the target entity elements will be included in the new group.
Specifies whether you wish to overwrite the group if it already exists, otherwise you will be prompted for overwrite permission is the group already exists.
The default name for the new group to be created will be
Fbdy_Group
.
Change it if desired.
Press this button to actually make the group.
This will remove any freebody plot from the graphics screen.
This will reset all widgets to their default values and will remove any plot.
When Apply is pressed, the display will update using the new entities and will retain whatever results and display attributes have been selected previously.
Important:
Once a target entity has been selected, it will remain the target entity for the freebody plot until the user physically changes it or he changes the
Action/Object/Method or presses the Default or Reset buttons. This will reset the target entities selection to its default and clear the plot.
11
220
PART 6
Results Postprocessing
11
12.4
Display Attributes
Freebody plots can be displayed with various attributes. Display attributes for freebody plots area accessible by pressing the Display Attributes selection button on the Results application form with the Object set to Freebody. It is not required to use this option. Appropriate defaults will be used.
Toggles the form to change display attributes for freebody plots.
The following table describes in detail the freebody display attributes which can be modified:
Show:
Attribute
Display As:
Dimensions:
Color/Components
Display Free Edges
Only
Display Nodal
Contributions
Scale Arrows /
Constant
Length
Hide Results Near
Zero
Description
For freebody plots you can display Forces, Moments, or Forces and
Moments simultaneously. This is also true for interface loads. For forced displacement plots these choices are Translational,
Rotational or both simultaneously.
For all three types of freebody plots, the resulting vectors can be plotted as either components or resultants.
This option is an easy way to display only the components that you want. By default, vectors in three dimensions will be displayed. You can constrain this to particular planes with respect to the global coordinate system. Only those components will be displayed or, if a resultant display is requested, the resultant will be calculated with respect to that plane only.
You can turn ON or OFF the display of any component or resultant and change their colors with these toggles and color widgets.
Only vectors of freebody or forced displacement plots on free edges of the model will be displayed if this toggle is ON. This essentially will eliminate any internally applied loads or internal reaction loads from the display. This type of display will not work for bar element models.
For Interface Loads only the contributions from each individual node can be plotted simultaneously as well as the total interface load if this toggle is turned ON.
If the Scale Arrows toggle is turned ON then vector lengths will be scaled relative to one another based on their magnitudes. Constant will keep all vector arrows the same length. Both are scaled relative to the a percentage of the screen size.
This is a scale factor to be applied for sizing the vector arrow lengths. By default it is set to 10% of the screen size.
If you wish to see all results whether they are zero or not, turn this toggle OFF.
CHAPTER 12
Freebody Plots
221
Attribute
Zero Tolerance
Display Values
Exponential /Fixed
Significant Digits
Display Title
Color / Title
Font / Location
Automatic Print
Text Report
Append
Display via Session
File
Reset Plot
Defaults
Description
Sometimes it may appear that some vectors of the freebody plot are not being displayed. This could be because the Hide Results Near
Zero toggle is ON and the Zero Tolerance is set too high. Change this tolerance if necessary to view or not to view vectors below this gate value.
Turn this toggle ON or OFF depending on whether you wish to see the values associated with the vector. You also have control of the display of these values.
Values on vectors can be displayed as either fixed (real) values or in exponential form.
You may also set the number of significant digits of the vector label values.
Turn this title on if you wish to display a title with the plot. For more versatile title display, use the Titles utility from the main
Titles
(p. 284) in the MSC.Patran Reference Manual, Part 1: Basic
Functions.
Titles can be colored and specified in the textbox. If no title is supplied but the Display Title toggle is ON, a default title will appear.
You may create a title to display in the upper or lower left corners of the screen and specify the font size.
When toggled ON, a hardcopy print command will be generated and sent to the currently selected printer definition under the Print application. If multiple results are selected, then multiple plots will be sent. This does not work when MSC.Patran is run in batch mode with no graphics.
If this toggle is turned on the data associated with this plot will be dumped to a file called
<db_name>_freebody_data.dat
.
If this toggle is ON then the text report will append to any already existing file.
This option will put the session file call to create the freebody plot in the MSC.Patran command line. The plot will not be created until you issue a RETURN from the keyboard with the cursor control in the command line. This is useful if you wish to look at multiple plots sequentially. Select all the Result Cases and/or subcases and/or result types, then turn this toggle on. Each time you want to see the subsequent plot press the RETURN key when the focus is in the command line. This will also create a session file called
<db_name>_play_freebody.ses
.
This will remove any freebody plot from the graphics screen.
This will reset all widgets to their default values and will remove any plot.
11
222
PART 6
Results Postprocessing
When Apply is pressed, the display will update using the target entities and results which have been selected previously and the new display attributes. Defaults will set the form back to its default settings and Reset Plot will erase the vectors from the screen.
Important:
Once display attributes have been selected, they will remain in effect for the freebody plot until the user physically changes them or the
Action/Object/Method is modified.
11
CHAPTER 12
Freebody Plots
223
12.5
Create Loads or Boundary Conditions
This is the portion of the Freebody plot tool that saves the displayed data as load or boundary condition sets. It is not necessary to use this option unless you wish to create them from the
Freebody, Interface, or Displacement plots.
Toggles the form to create loads and boundary conditions from freebody plots.
Creating loads and boundary conditions from freebody plot displays is a two step process. First a field is created for the appropriate type such as force, moment, or displacement. Then the fields are assigned to a Load Case. Only what is graphically displayed on the screen is actually created in the fields. The following table explains each option.
Attribute Description
Create
Force/Moment
Displ/Rotational
Field
Create both a force and a moment field or one or the other
(translational and rotational fields for forced displacements). What is displayed graphically is what is created in the new field. You must create at least one field in order to create a load set. Once fields are created you may use them as you would any other field.
Then access them and modify or delete them from the Fields application. The fields are created in the coordinate system specified as the transformation coordinate on the main (Select
Results) form, otherwise they will be written in the global system.
For Interface loads, the display attribute “Display Nodal
Contributions” must be on in order to create fields for this type of plot.
Assign Fields to LBC
Toggle ON to assign the fields to a new LBC set (load set). Then enter a name and assign it to a load case. Once a load set has been created you may access, modify, or delete it from the Loads/BCs application. The same naming convention is used here as is used when creating fields. If the Type is Interface Loads, then only this option is presented since only at a single node will force and moments be created. No fields will be created. Therefore, no fields are necessary.If you wish you may assign a new load case name and a new load case will be created. For Interface loads only the
“Total Load” is assigned to the LBC, not the fields.
Overwrite / Increment
When multiple results are selected for display, multiple fields and
LBC set names will be created. The names of the fields and LBC set names will be augmented by appending a version on the end of them if Increment is selected (e.g., Fbdy_Force.001,
Fbdy_Force.002, etc.). You can overwrite or increment the names.
Field Name
LBC Name
Load Case
Assignment
The default name for a field is
Fbdy_<type> where the type can be
Force, Moment, Translation, or Rotation. Change it if desired.
The default LBC name is
Fbdy_LBC
or
Fbdy_Disp_LBC
. Change it if desired.
When creating a new LBC you can select to which Load Case it is assigned from this listbox. The default is the Default load case.
11
224
PART 6
Results Postprocessing
Attribute
Insert / Increment
LC Name
Reset Plot
Defaults
Description
This works similar to Overwrite/Increment with field names. For
Load Case names however the option is to either insert the new
LBC into the currently selected Load Case or to create a new Load
Case with the name incremented with a version number (e.g.,
LBC.001,LBC.002, etc.).
You can type in a new Load Case name here is you wish or select an existing one from the Load Case Assignment listbox.
This will remove any freebody plot from the graphics screen.
This will reset all widgets to their default values and will remove any plot.
Pressing Apply here will create the specified fields and load set for the currently displayed plot for access and assignment in a subsequent finite element analysis. Defaults will set the forms back to their default settings and Reset Plot will erase the vectors from the screen.
Some consideration to be aware of when creating fields and LBC sets.
•
If a planar display is plotted of three dimensional data, then the appropriate column is zeroed in the field.
•
The display attribute “Display Free Edges Only” can limit the amount of information that is placed in a field for Freebody and Displacement plots.
•
The display attribute “Display Nodal Contributions” for Interface loads must be on in order to create fields. Only the “Total Load” will be written to the new LBC set, not the fields.
•
The display attribute “Hide Results Near Zero” affects the amount of data written to the fields for Freebody Loads and Interface Loads but not Displacement. All displacement data is written no matter how small since all the data is necessary for a re-analysis. Zero displacement is a necessary boundary condition.
•
Once a new LBC is created or an existing one is modified, you must make sure that the
LBC is the current LBC in order to visualize the LBC markers on your model. This is done in the Loads/BCs application.
11
CHAPTER 12
Freebody Plots
225
12.6
Tabular Display
The Show Spreadsheet icon on the Freebody plot tool accesses a spreadsheet.
Pressing this button icon makes the freebody spreadsheet appear.
This spreadsheet will fill itself with result values for each node that has a vector plot summarizing the loads or displacements whether they be internal, reaction, applied or other. It also summarizes the totals for equilibrium checks and other purposes. Only the nodes of the currently displayed freebody plot will be reported in the spreadsheet. Also the spreadsheet will be cleared and redisplayed each time a new plot is created. You may bring up and close down the spreadsheet and the data will remain intact until a new plot is created.
The Node number is reported in this column. The same node may appear more than once if more than one load type is associated with it.
The two Force and Moment resultants and each component are reported in the spreadsheet independent of what is displayed on the screen.
Type refers to the load type for the particular node that is reported. Type can be Applied
Load, Reaction Load, Internal Load, or Other load. Other load refers to the fact that the
Total load is other than zero, therefore some unaccounted load contribution exists for that node.
1
6
7
8
9
2
3
4
5
Node Force Moment Fx Fy Fz Mx My Mz Type
The labels on the spreadsheet above will change to displacements when the Forced
Displacement method is displayed.
The totals for each component are reported at the bottom of the spreadsheet. When Freebody
Loads are plotted on the graphics screen, these totals should be zero (equilibrium should exist).
If not, then other unaccounted load contributions must exist, such as those from rigid element,
MPCs and externally coupled stiffness matrices. You may also click the mouse on each cell to get more detailed information in a text box below the spreadsheet. Also if the Method is set to
Interface Loads, contributions from all nodes specified as target entities will be displayed even though graphically only the summation point displays the vector plot.
A Report button is also available from this spreadsheet that will write its contents out the a file called
<db_name>_freebody_data.dat
where
<db_name>
is the name of the database.
11
226
PART 6
Results Postprocessing
11
A special utility PCL function can be used in conjunction with the freebody spreadsheet to interact in almost any way imaginable. If you define the function below and compile it into
MSC.Patran with a
!!input <function_name>
before the spreadsheet is opened, then anytime you click on a cell in the spreadsheet this call back function is called. Please see
The PATRAN
Command Language (PCL) Introduction
(p. 5) in the PCL and Customization for details on how to program in PCL.
freebody_spreadsheet_cell_cb
(spreadsheet_id, textbox_id, segment_id, from_column, from_row, to_column, to_row)
Description:
This is a call back function that is called anytime a cell or group of cells is selected in the freebody spreadsheet. The arguments to the function are all inputs supplied by the callback function of the spreadsheet. The function must be defined by the user and compiled into
MSC.Patran before the freebody spreadsheet is opened. The contents of this function are left up to the user’s imagination.
Arguments:
WIDGET spreadsheet_id
WIDGET
INTEGER
INTEGER
INTEGER
INTEGER
INTEGER textbox_id segment_id from_column from_row to_column to_row
This is the widget ID of the spreadsheet. Knowing the widget ID you have full control over it and can make modification to the spreadsheet such as adding or removing rows or columns.
This is the widget ID of the textbox on the bottom of the form under the spreadsheet. Knowing the widget ID of the textbox you have full control over it such as adding and removing text from the textbox.
This is the graphics segment ID. Knowing the segment ID into which the freebody plot has been graphically written
(the vectors and labels) you have full control over them such as deleting, modifying or adding to the graphics already in that segment.
This is the first column in the range of selected cells from the spreadsheet.
This is the first row in the range of selected cells from the spreadsheet.
This is the last column in the range of selected cells from the spreadsheet.
This is the last row in the range of selected cells from the spreadsheet.
Example.
A good example of usage of this PCL utility is the highlighting of nodes when a cell or range of cells is selected. For example, say that you wish to know graphically which node a particular value in the spreadsheet referred to.
Although the node ID is indicated in the spreadsheet, with a little programming, a user could create a function that when a cell or cells are selected, the corresponding node(s) is/are highlighted graphically on the screen.
CHAPTER 12
Freebody Plots
227
12.7
Examples of Usage
The following example illustrates the basic usage of the Freebody plot application.
represents a continuous truss structure subject to a vertical end force and gravity force at the center of gravity. The structure is fixed to a wall. The goal is to run a static analysis and to determine and graphically display the reaction loads experienced at the wall, and to cut the structure at any point and display a freebody diagram as well as display the internal loads at various locations. Also a subsequent detailed analysis is required at one of the joints, therefore the internal loads need to be saved as a load case set.
An MSC.Nastran analysis is performed with a Case Control statement requesting a Grid Point
Force Balance table: GPFORCE = ALL. The applied loads are shown as displayed by the Results
Freebody application. The resulting OUTPUT2 file is imported into the MSC.Patran database.
23.50
12
12
9.810
Figure 12-1 Example Plot of Applied Loads for the
Continuous Truss Example
Display the Applied Loads from the Model
1. Set the Action to Create, the Object to Freebody and the Method to
Loads.
2. Make sure the Select Results button icon is selected (Method = Load).
3. Select a Result Case (and a subcase if one exists).
4. Select the result type Applied Loads from the Result Type listbox.
5. Press the Apply button to display the nodal equivalenced applied loads.
6. To change any display attributes of the vector plot, press the Display
Attributes button icon. Press the Apply button again to affect any additional changes.
In
, the two nodal forces appear. The gravity load in this case is concentrated at a single node. Had the gravity load been applied as a MSC.Nastran GRAVity force, equivalent nodal forces would have been distributed at all node points. In this case it was not necessary to select Target Entities. The whole model was used by default.
11
228
PART 6
Results Postprocessing
Display the Reaction Forces from the Model
1. Set the Action to Create, the Object to Freebody and the Method to
Loads.
2. Make sure the Select Results button icon is selected (Method = Load).
3. Select a Result Case (and a subcase if one exists).
4. Select the results type Reaction Loads from the Result Type listbox.
5. Press the Apply button to display the nodal equivalenced reaction loads.
6. To change any display attributes of the vector plot, press the Display
Attributes icon. Press the Apply button to affect any additional changes.
Again, the entire model was used as the default display. No target entities were selected in
33.31
112.1
107.1
107.1
107.1
Figure 12-2 Example Plot of Reaction Loads at the Wall for the Continuous Truss
Example. Both Resultant and Component Displays are Shown.
11
CHAPTER 12
Freebody Plots
229
Display a Freebody Diagram
1. Set the Action to Create, the Object to Freebody and the Method to
Loads.
2. Make sure the Select Results button icon is selected (Method = Load).
3. Select a Result Case (and a subcase if one exists).
4. Select the results type Freebody Loads from the Result Type listbox.
5. Press the Target Entities button icon, and select target entities as required. If this step is skipped the entire model, or whatever is currently posted will be used as the target entities. If the entire model is used, only applied and reaction loads will be displayed.
6. Press the Apply button to display the freebody diagram plot.
7. To change any display attributes of the vector plot, press the Display
Attributes button icon. Press the Apply button to affect any changes.
Apply
23.50
23.50
33.31
107.08
9.81
107.08
112.14
107.08
9.81
Figure 12-3 Example Plot of the Total Freebody Diagram for the Continuous Truss
Example. Both Resultant and Component Displays are Shown.
11
230
PART 6
Results Postprocessing
View the Internal Loads at a Node or Nodes
1. Set the Action to Create, the Object to Freebody and the Method to
Loads.
2. Make sure the Select Results button icon is selected (Method = Load).
3. Select a Result Case (and a subcase if one exists).
4. Select the results type Internal Loads from the Result Type listbox.
5. Select the Target Entities button icon and select target entities as required. This is required for internal load display unless only a portion of the model is posted via groups.
6. Press the Apply button to display the internal loads plot.
7. To change any display attributes of the vector plot, press the Display
Attributes button icon. Press the Apply button to affect any changes.
Apply
23.50
23.50
107.08
33.31
107.08
9.81
107.08
112.14
9.81
Figure 12-4 Example Plot of Internal Loads for the Continuous Truss Example. Both
Resultant and Component Displays are Shown.
11
CHAPTER 12
Freebody Plots
231
Create a Load Case Set for Use in a Subsequent Analysis
1. Set the Action to Create, the Object to Freebody and the Method to
Loads.
2. Make sure the Select Results button icon is selected (Method = Load).
3. Select a Result Case (and a subcase if one exists).
4. Select the appropriate result from the Results Type listbox of which you would like to create a load set.
5. Press the Apply button to display the internal loads plot.
6. Press the Save Data button icon.
7. Enter a field name for the forces, a field name for the moments, a load set name or assign them to an existing load case. Or you can simply accept all the defaults.
8. Press the Apply button. Loads and fields will be created for whatever results type is currently displayed on the screen.
The newly created fields and load set can be modified, viewed, deleted or otherwise manipulated from the Field and Loads/BC applications respectively. They can also be re-assigned to other load cases via the
Loads/BC and Load Cases applications.
View the Vector Values on the Nodes Tabularly
1. Display the desired plot graphically (freebody, applied, reaction, internal, other) as explained in previous examples.
2. Bring up the spreadsheet by pressing the Show Spreadsheet icon. The results (resultants and components) for the current plot will be displayed in the spreadsheet for the target entities.
Apply
Apply
11
232
PART 6
Results Postprocessing
Display the Total Interface Load Across a Boundary
1. Set the Action to Create, the Object to Freebody and the Method to
Interface.
2. Make sure the Select Results button icon is selected (Method =
Interface).
3. Select the Result Case and subcase if necessary and Freebody Loads as the Result Type.
4. Select a node or location to act as the Summation Point or accept the origin as the default.
5. Select target entities. Press the Target Entities icon. The target entities must be all the nodes along an interface boundary for which you are interested in calculating the total load. In addition you must select the element on one side or the other of the nodes that define the interface line. This is a two step process. You must first select the nodes by changing the Select By pull-down menu to Node, select the nodes, then change the pull-down to Element, and select the elements.
6. Set the display attributes to show what you want (Forces/Moments,
Resultants/Components) if desired. Press the Display Attributes button icon to do this.
7. Press the Apply button. A single component vector will be displayed on the screen.
In
, we have selected nodes 3 and 1 to be the interface line.
There are element contributions from elements 3, 20, and 7, therefore these elements must be also selected as target entities. The summation point is node 2. A single vertical force of 23.5 and z-moment of 94.0 are the total interface loads experienced internally by cutting the model at this interface boundary.
Apply
11
23.50
3
2
1
3
20
7
94.00
Figure 12-5 Example Plot of Applied Loads for the Continuous Truss Example
CHAPTER 12
Freebody Plots
233
Create a Forced Displacement Boundary Condition
1. Set the Action to Create, the Object to Freebody and the Method to
Displacement.
2. Make sure the Select Results button icon is selected
(Method=Displacement).
3. Select the Result Case and subcase if necessary.
4. Select target entities if necessary. Press the Target Entities button icon.
Only elements or groups containing elements need be selected. The default is use all elements posted to the current viewport.
5. Set the display attributes to show what you want
(Translational/Rotational, Resultants/Components) if desired. Press the Display Attributes button icon to do this.
6. Press the Apply button. Component or resultant vectors will be displayed on all exposed nodes of the freebody (along the free edges of the model) by default.
7. Press the Save Data button icon.
8. Enter a field name for the translational displacements, a field name for the rotational displacements, and a load set name or assign them to an existing load case. Or you may simply accept all the defaults.
9. Press the Apply button. Enforced displacement boundary conditions and fields will be created for the currently displayed plot on the screen.
The newly created fields and load set can be modified, viewed, deleted or otherwise manipulated from the Field and Loads/BC applications respectively. They can also be re-assigned to other load cases via the
Loads/BC and Load Cases applications.
Apply
11
234
PART 6
Results Postprocessing
11
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
13
Insight
■
Overview of the Insight Application
■
■
236
PART 6
Results Postprocessing
12
13.1
Overview of the Insight Application
The Insight application provides capabilities for interactive results postprocessing. Insight is object oriented, providing postprocessing tools which are created, displayed, and manipulated to obtain rapid insight into the nature of results data. The imaging is intended to provide graphics performance sufficient for real time manipulation. Performance will vary depending on hardware but consistency of functionality is maintained as much as possible across all supported display devices.
The Insight visualization tools remain in the database and provide the means for results manipulation and review in a consistent, easy to use manner. The available tools include
Isosurfaces, Streamlines, Streamsurfaces, Contours, Tensors and others described in detail in this chapter.
Definitions
Tool Definitions.
Insight provides thirteen different tools for results visualization. These tools allow you to graphically examine your analysis results using a variety of imaging techniques.
Insight allows for the simultaneous display of multiple tools to aid in the understanding of interactions between results. This section will provide a basic understanding of the different tool types which you will create and manipulate using the Insight application.
The following table summarizes the tools available in Insight followed by a detailed description of each.
Isosurface
Streamline
Streamsurface
Threshold
Fringe
Contour
Element
Tensor
Vector
Marker
Value
Deformation
Cursor
Surfaces of constant result or coordinate value.
Tracing of a particle path (or paths) through a vector field.
Surfaces generated along streamlines displaying a vector field’s vorticity as a ribbon along a streamline.
3-dimensional contour surfaces through solids.
Contoured bands of color representing ranges of results value.
Lines of constant result value.
Element-based polygon-fill or wireframe plot with color representing results values.
Tensors are depicted at the result locations as three dimensional cubes or squares with vectors showing direct and shear components.
Vector plot of result components or resultants.
Colored scaled symbols representing scalar results.
Annotation representing the actual result value displayed at the result location.
Displays the model and posted tools in a deformed state.
Displays result values at nodes/elements selected with the left mouse button and optionally loads these values into a spreadsheet.
CHAPTER 13
Insight
237
Isosurfaces
are surfaces of constant value. The constant value may be based upon either a scalar nodal-averaged result or a constant coordinate value. Coordinate-based isosurfaces may be defined in either the global cartesian (cid=0) system or in any alternate coordinate system
(cartesian, cylindrical or spherical). An isosurface tool may be defined as a single surface at a constant value (isovalue) or a series of up to five surfaces uniformly distributed between a high and a low value. Other tools may be targeted at isosurface tools and they will update accordingly as the isosurfaces are manipulated in the
form. Isosurfaces may also be used to clip the displayed model. The portions of the model which are greater than and/or less than the isovalue(s) may each be displayed as None, Transparent, Free Edge, Wireframe, Shaded, or
Hidden Line. These clipping attributes allow for displays such as a shaded model only where a result value exceeds a specified amount (e.g., display all the volume which exceeds the allowable stress).
Streamlines
are a tracing or set of tracings of particle paths through a vector field. They are associated with nodal vector data. They emanate from nodes defined by a database entity called a rake. A rake is referred to by its name; a user-definable string identifier. Each rake defines a list of nodes or node pairs for stream entities. A streamline’s color may be set to a fixed value or mapped to display the magnitude of the vector field along the stream path. Other tools may be targeted at streamlines. These tools will be visualized along the streamline(s) and will update as the streamlines are manipulated.
Streamsurfaces
are surfaces generated as a ribbon along a streamline. They are associated with nodal vector data. Other tools may be targeted at a streamsurface or set of streamsurfaces defined by a streamsurface tool. Streamsurfaces permit you to visualize vortices in fluid flow problems.
Threshold
tools are 3-dimensional contour surfaces. They are associated with nodal scalar data.
As contour lines depict the lines of constant value on surfaces, thresholds depict the surfaces of constant value through solids. Each individual threshold within a threshold tool is an isosurface.
Unlike the isosurface tool, thresholds are not a targettable tool nor can they be used to define a clipping surface. Thresholds are controlled by the current range levels and spectrum definition for color, number of displayed surfaces, and surface values.
Fringe
tools map color to surfaces or edges based on the result data defined for the tool. Fringes are developed from nodal-averaged scalar values. Fringes may be targeted at the model’s element faces or free edges or to previously created isosurfaces, streamlines, and streamsurfaces.
The fringe tool will supersede all existing or default color definition for the entity at which the fringe is targeted. The fringe tool also supports transparency.
Contour
tools display lines of constant results value on surfaces. As with thresholds, the current range and spectrum definition control the number of contours, contour location, and contour color. Contours are based on nodal-averaged scalar values. The contour tool displays lines of constant results values whereas the fringe tool displays ranges or bands of results value.
Contour line displays are useful to create a hardcopy image of the Insight viewport on a black and white hardcopy device.
Element
tools display elements as polygon fills or wireframe with color mapped to each element by a single (assigned) results value. Element tools are based on element centroidal scalar data.
Element tools may be targeted at model elements or isosurfaces. Isosurface-targeted element tools will display the elements which traverse the targeted isosurface(s).
12
238
PART 6
Results Postprocessing
12
Tensor
tools display an iconic representation of a symmetric stress tensor. Tensors may be oriented in the axes of principal stress or the tensor’s defined coordinate system. Tensors may be defined by element- or nodal-based tensor data. Nodal tensors are mapped from element tensors and are used when a tensor tool is targeted at other tools. Tensors may be targeted at nodal- and element-based model features as well isosurfaces, and streamline tools.
Vector
tools display nodal or element based vector data as component or resultant vectors.
Vectors may be colored and scaled based on magnitude and may be targeted at model features, isosurfaces and streamlines.
Marker
tools display nodal or element based scalar results as icons at the result locations. The icons may be scaled and colored based on the assigned data. Icons shapes may be a triangle, square, diamond, hourglass, cross, circle, dot, point, sphere, or cube. Markers may be targeted at model features, isosurfaces and streamlines.
Value
tools display the data values of nodal- or element-based scalar results as text at the results locations. The value text color may be fixed to a value or mapped based on the results data, the current range and spectrum definitions. Values may be targeted at model features, isosurfaces, and streamlines.
Deformation
tools are used to display the current model and posted tools in a deformed state.
Only one deformation tool may be posted at a time and the tool will modify the display of the posted model and all posted tools. An optional display of an undeformed model is controlled as an attribute of the deformation tool. The targeting of deformation tools is not controllable since they will have global effects. Deformations may be used to display any nodal vector data as a deformation.
Cursor
tools are used to display result values and load result values into a spreadsheet using the cursor. Pressing the left mouse button will select the nearest node or element and display the value of the assigned result on the screen. Holding the mouse button down and dragging it will interactively move the displayed value or id to represent the current entity closest to the cursor.
The selected entity ids and results will also be added to the cursor tool spreadsheet for review, sorting and output to a text file.
The Insight application provides the means of Creating, Modifying, Deleting, Posting and
Unposting these tools as well as means for dynamically manipulating these tools for interactive results imaging. Each tool created has assigned attributes which determine its characteristics. All tools have the following attributes.
Name
Type
Result(s)
Target
Display Attributes
Animation
Attributes
Posting Status
A unique user-definable string descriptor to identify the tool.
One of the thirteen tool types described above.
A list of load cases and a corresponding result which the tool is to display. A coordinate based isosurface would refer to a coordinate frame and axis versus a result.
Where the tool is to be displayed. This is either on a model feature or on a targettable tool (isosurfaces, streamlines, streamsurfaces).
Each tool type has specific settings to control how the tool type is to be displayed.
Attributes to describe whether the tool is to be animated and how the results are to be mapped to animation frames.
Each tool is either Posted (displayed) or Unposted (not displayed).
CHAPTER 13
Insight
239
Tool Targets.
Insight tools may be targeted at selected model entities or selected tools. The model based targets may be defined by a list of posted groups or by all posted entities. The model entities and tools which may act as targets for Insight tools are described:
Elements
will generally be displayed through the model. For example, an isosurface targeted at the model’s elements will be displayed as a plane passing through the model orthogonal to some coordinate system axis.
Free faces
describe those element faces common to only one element. This includes faces lining the outside surface of a model or those inside surfaces exposed to internal voids. Free faces are appropriate targets for displays such as fringe plots which are normally displayed on the surface of the model or on a cutting plane through the model.
All Faces
display results on each face of each element.
Free Edges
display results on edges common to only one element. Use this target type when you wish to display results on the same edges which are used to draw the model when Free Edge is selected as the display method in the Preferences-Insight... form.
All Edges
display results on all element edges. Using this target selection allows you to map results onto a wireframe representation of the model.
Nodes
display the selected tool’s result at each nodal location of the model. Tensor, vector, marker and value tools may all be displayed at nodal locations.
Corners
display the selected tool’s result at nodes which are common to only one element.
Tensor, vector, marker and value tools may all be displayed at corner locations.
Isosurfaces
are selectable tools. The isosurface can be used as a target for fringes, contours, tensors, elements, vectors, markers, and values, as well as being a visualization tool by itself. A tool posted on an isosurface will be displayed on its calculated surface(s) of constant value
(coordinate or result).
Streamlines
are selectable tools. Fringes, tensors, vectors, markers and values may be targeted to streamline tools.
Streamsurfaces
are selectable tools for fringes and contours.
The following table summarizes the valid targets for all tools.
12
TOOL
Isosurface
Streamline
Streamsurface
Threshold
Fringe
Contour
•
•
•
•
•
•
•
•
• • •
•
• •
•
240
PART 6
Results Postprocessing
12
Element
Tensor
Vector
Marker
Value
Deformation
Cursor
Other Definitions
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Named Posting
Post
Unpost
A user defined grouping of tools to be displayed simultaneously.
To display the entity.
To remove the entity from the display.
Range
Viewport Range
Auto Range
Rake
A MSC.Patran database entity defined by a number of levels and
(1-12 for Insight) and a series of threshold values for each level within a range. Ranges are used to map spectrum colors to results values. A spreadsheet form is available to control range levels.
The range entity currently assigned to the Insight viewport.
A range which is not a database entity but is automatically calculated for a tool based on the results values. This type of range may be manipulated dynamically to change the range extremes and the number of intermediate levels.
A database entity which describes a list of nodes. A rake entity is needed for Streamline and Streamsurface tools.
Reduced Rendering
A graphical rendering style available to eliminate surface rendering while performing various tasks with Insight. Reduced Rendering will display only vector outlines for all filled faces. This is useful for manipulating large models or for increasing speed on machines without hardware shading. This capability is controlled from the
Insight Preferences form.
CHAPTER 13
Insight
241
Capabilities and Limitations
Insight provides the capabilities of the following actions, and the capability to manipulate results visualization tools as well as view the finite element model.
❏
❏
❏
❏
Dynamic control is provided for moving isosurfaces through the model, manipulating the color/range assignment for tools, and for controlling and creating animations of static and transient results. The forms controlling this functionality are described in
Results are selected from the database and assigned to tools using simple forms. Results transformations are provided to derive scalars from vectors and tensors as well as to derive vectors from tensors. This allows for a wide variety of visualization tools to be used with all of the available results. Result transformations include component extractions as well as
calculations such as magnitude, vonMises stress, or maximum principal vector (see
The Insight imaging routines are optimized for graphical speed. You should be aware of the following limitations:
•
With the exception of element targeted fringe tools, results will be displayed as nodal averaged or element centroidal data. Other result types will be averaged prior to display.
•
The combination of results and the manipulation of loadcases for display is not available in Insight. Insight will only access results currently residing in the database.
Combined and derived results cases can be created in the Results application within
MSC.Patran. Refer to
(Ch. 11), for more information.
12
242
PART 6
Results Postprocessing
12
13.2
Using Insight
The Insight application is based on the creation and manipulation of results visualization tools.
The first action to be performed using Insight is to create a tool. This is done using the
Creating a tool involves five basic steps:
1. Select a tool type from the
2. Select a result from the
form, or (for an isosurface) select a
Isosurface Coordinate Selection
(p. 253) form. For an isosurface,
this step requires both selecting result data or a coordinate axis and specifying an initial value for the data. An isosurface tool can either be tied to a single value or span a range of values using two, three, four, or five equally surfaces.
3. Set the tool attributes using the applicable
4. Select the target for the tool from the
(p. 239) pull-down menu in the
Insight Imaging form.
5. Press the Apply button on the Insight Imaging form. The tool will be displayed.
Once a tool has been created, it may be modified using the
action on the Insight
Imaging form. To modify a tool, first select the tool from the Existing Tool listbox, modify as needed, and click the Apply button to update the display.
Multiple tools may be created and posted simultaneously. One of the most common uses of multiple tools is to first create an isosurface, then create a fringe tool targeted to the isosurface.
This tool combination will display a surface of constant coordinate or scalar result which is colored with a fringe contour of some other result. The isosurface could, for example, display a surface where vonMises Stress = 10,000 psi, while the surface is displaying a fringe of maximum principal strain. Or, an isosurface of constant global X could be created and a fringe of temperature created and posted to it.The combinations of superimposed tools are virtually endless. All displayed tools are updated as their targeted tools are moved or modified.
You can display a deformed shape with a tool as well. Creating and posting a deformation tool will display all posted entities in a deformed state.
Once a tool or set of tools has been created and posted, capabilities for moving isosurfaces, creating animations, manipulating the range and color assignment, and posting and unposting existing tools are accessible through the
menu on the MSC.Patran main
form. Tools already created may be posted or unposted using the
form, which is accessible by selecting the Post/Unpost Tools option in the Insight Control menu.
Posted isosurfaces may be moved by manipulating the value(s) defining the tools. This capability is provided through the
(p. 267) form, which is accessible by
selecting the Isosurface Control option in the Insight Control menu. A posted isosurface is selected from the listbox as the active surface to control. The surface can be moved using the slidebar or by entering a value in the databox. The Start value applies to all isosurfaces. The End value is used if the isosurface tool was created with multiple surfaces (a maximum of five is allowed). The speed at which an isosurface will respond to the slidebar is dependent on the size of the model, the speed of the display device, and the current slidebar resolution which is set in
(p. 278) form. The Insight Preferences form is accessible by
selecting the Insight option in the Preferences menu on the MSC.Patran main form.
CHAPTER 13
Insight
243
Selecting and manipulating the active range tool is done in the
form, which is accessible by selecting the Range Control option in the Insight Control menu. Although many tools may be displayed simultaneously, only one spectrum and range is available for display. Any one of the posted tools may be selected as being the active range tool; i.e., the tool which is associated with the displayed range and spectrum. The other tools posted may be color coded to show a gradation of results data but may not necessarily be tied to the active range.
The ranges and color assignment for the active range tool can be defined using two methods;
Auto and Viewport. An option on the
(p. 268) form is used to select the desired
method. The Auto method is used if the range is to be automatically calculated based on the result assigned to the active range tool, or if you wish to dynamically manipulate the range values or number of levels using the slidebars on the Range Control form. The Viewport range method uses the MSC.Patran range assigned to the Insight viewport. MSC.Patran ranges are created and manipulated using
Display>Ranges
(p. 307) in the MSC.Patran Reference Manual,
Part 1: Basic Functions, which is accessible by selecting the Ranges option in the Display menu on the MSC.Patran main form. The Viewport range provides greater user control for range levels but cannot be used for dynamic range manipulation.
The other posted tools can have color assigned using three methods: Auto, Viewport, and
Active. Auto will automatically show color spanning the current spectrum for each tool regardless of the current range levels. This method is good for understanding qualitative result levels for all tools, but colors assigned will not correspond to the displayed spectrum levels.
Viewport will assign colors based on the Viewport range. The Active tool range method will guarantee that all tools displayed map to color range levels as displayed. Adjusting the slidebars on the Range Control form will dynamically update the display as the values are modified.
Animations are setup and controlled using either the
Modal Animation form which are accessible from the Insight Control menu.
The Modal Animation form provides for rapid access to a modal animation display with minimal user interaction. You need only to select a vector result and press the animate button.
A wireframe display of the selected result’s deformed shape will be animated using a sinusoidal variation of scale.
The Animation Control form provides access to all of the animation functionality provided by
Insight. Its
(p. 270) form allows for the modification of the posted tools as
needed to set the animation attributes. All posted tools will be displayed during an animation but only those tools with the animation enabled will change from frame to frame. Animation frames are created by mapping the tool results onto a requested number of animation frames.
Each posted tool enabled for animation may be animated using a global variable for transient results (more than one load case assigned to the tool) or using a ramp or sinusoid scaling for static results (only one loadcase used). Linear interpolation is used for mapping transient results to animation frames. Once an animation has been created and is being displayed, the Animation
Control form provides capabilities for cycling and stepping through the animation sequence.
12
244
PART 6
Results Postprocessing
12
13.3
Insight Forms
The Insight forms used to create and modify imaging tools are described in detail in the sections titled
(p. 254). Capabilities for control and
manipulation of the Insight viewport and tools are accessed through the forms described in the sections
(p. 276). These forms are accessible
through the Insight pull-down menu on the MSC.Patran main form.
Insight Imaging
The Insight Imaging application form provides the capabilities to Create, Modify, and Delete tools. Additional forms for selecting results for tools (or coordinate axes for isosurfaces) and for controlling display attributes are accessed from the Insight Imaging form during the Create and
Modify actions.
❏
❏
❏
This action is used to create Insight visualization tools.
This action is used to modify existing Insight visualization tools.
This action is used to delete existing Insight visualization tools.
❏
Results Attributes This form is accessed from the Results Selection button on the
Insight Imaging form. This form is used to create a result based tool.
❏
This form is accessed either from the Select Results form or the
Animation Setup form. Animation attributes are assigned to a tool as part of its definition. Each tool may have its own unique animation attributes to control how each tool is handled during animations.
❏
This form is accessed from the Results Selection form after a Load case(s) and result is selected. This form is used to define more details regarding the selected result such as selecting a transformation method if the result must be transformed, selecting a layer if multi-layered results data exists, and selecting a default loadcase if multiple load cases are selected.
❏
This form is accessed from the Results Selection form for result based isosurfaces. The initial result value(s) for the isosurface and the number of surfaces for the isosurface tool are defined through this form.
❏
This form is used instead of the Results Selection form for coordinate based isosurfaces. An isosurface can be tied to any axis of a user defined coordinate frame or the global system (frame 0).
The initial coordinate value(s) and number of surfaces for the isosurface tool are also specified in this form.
❏
There is a unique Attributes form for each tool type. Each tool may have unique display attributes assigned. They are controlled from the Attributes form associated with the tool type.
CHAPTER 13
Insight
245
Create
Select Create from the Action pull-down menu to create new visualization tools.
Action:
Tool:
Insight Imaging
Create
Isosurface
Select a tool type. See
Tool Definition
Isosurface Name
Isos_1
Existing Isosurfaces
A default name is provided. If desired, enter a new name for the tool.
Existing tools of the same type will be listed here.
Select a tool from the list to copy its attributes to the new tool, if desired.
Select the Result or Coordinate option for an isosurface value. Select Scalar, Vector or Tensor for Cursor Tool Result type. These options will not be displayed for other tool types.
Isosurface Value
◆
Isosurface Attributes...
Post Tool on Apply
Posting Target Selection
Target:
Use All Posted
Target Groups group_1
Displays the applicable tool attributes form. See
Select this option to post the tool, if desired.
Select a target from the pull-down menu. See
Select this option to target the tool to the entire posted model versus the displayed portions of specific groups.
12
Select the desired group of tool names from this list to define the target, if not using all posted.
Apply
246
PART 6
Results Postprocessing
12
Modify
Select Modify from the Action pull-down menu to modify existing visualization tools.
Action:
Tool:
Insight Imaging
Modify
All Types Select a specific tool type to list in the Existing
Tools listbox. See
Alternatively, select All Types to list all existing tools.
Tool Definition
Tool Name
Existing Tools
IS-Isos_1
FR-Fringe_1
Enter the name of an existing tool to modify in the
Tool Name databox, or select a tool from the Existing
Tools listbox.
Isosurface Attributes...
Post Tool on Apply
Posting Target Selection
Target:
Use All Posted
Target Groups group_1
Displays the
Displays the applicable tool attributes form. See
Select this option to post the tool, if desired.
Select a target from the pull-down menu. See
Select this option to target the tool to the entire posted model versus the displayed portions of specific groups.
Select the desired group of tool names from this list to define the target, if not using all posted.
Apply
CHAPTER 13
Insight
247
Delete
Select Delete from the Action pull-down menu to delete existing tools.
Action:
Tool:
Insight Imaging
Delete
All Types
Select a specific tool type to list in the Existing Tools listbox.
See
(p. 254). Alternatively, select All Types to
list all existing tools.
Existing Tools
IS-Isos_1
FR-Fringe_1 Select tools from the Existing Tools listbox. They will be added to the Tools to Delete listbox.
12
Tools to Delete
Selecting tools displayed in the Tools to Delete listbox will return them to the existing Tools listbox.
Apply
Deletes the tools listed in the Tools to Delete listbox.
248
PART 6
Results Postprocessing
12
Results Selection
The following form appears when the Results Selection button is selected on the Insight Imaging form when Create or Modify is the selected Action.
Updates the results list based on the selected loadcase(s).
Select the Load Case(s) from the list to be associated with the tool. If multiple load cases are selected, a default load case is assigned using the Results Options Form. Only the default load case results will be displayed, except during an animation.
Results Selection
Current Load Case(s)
Update Results
Isosurface Result
1.1-Displacements, Translational
2.1-Applied Loads, Translational
3.1-Constraint Forces, Translational
4.1-Strain Tensor,
5.1-Stress Tensor,
OK
Displays
Cancel
Displays
Displays
(p. 252) to specify an initial isovalue and number of
surfaces for an isosurface tool type.
Select a desired result from this list. Only those results which are of the same type as the selected tool, or those that can be transformed to the tool’s result type, are listed. For example, a streamline tool displays vector results, therefore only vector and tensor result types will be listed. The transformation method for different type results is specified using the Result Options form. If the result has multiple layers defined, the layer to display is also selected from the Result Options form.
CHAPTER 13
Insight
249
Animation Attributes
The following subordinate form appears when the Animation Attributes button is selected on the Results Selection form.
Select this option to enable animation for the tool. All posted tools will be displayed during an animation, but only those that have been enabled will animate (i.e., change from frame-to-frame).
Animation Attributes
Enable Animation
Animation Type
Global Variable
Ramp
Sinusoid
Global Variable
Select an animation type.
Global Variable
is used to animate transient results through the load cases selected for the tool. This selection is only available for tools with more than one load case.
Ramp
is used to ramp the default load case result or coordinate isovalue multiplier from 0.0 to 1.0.
Sinusoid
is used to vary the default load case result or coordinate isovalue multiplier sinusoidally from -1.0 to 1.0.
12
Min.: 0.0
Max.: 1.0
OK Cancel
If the animation type selected is Global Variable, a variable must be selected. All global variables defined for the selected load cases will be listed as well as LOAD CASE
INDEX which may be selected to animate only the tool, versus the selected load cases.
250
PART 6
Results Postprocessing
12
Result Options
The following table provides additional definitions for the selected result transformation method.
Transform Type
Transform
Method
None
Description
Scalar to Scalar
Vector to Vector
Tensor to Tensor
No transformation is used if the result data type matches the tool’s data type.
Vector to Scalar Magnitude
X Component
Y Component
Vector magnitude.
1st vector component.
2nd vector component.
Z Component
3rd vector component.
Tensor to Scalar XX Component
XX tensor component.
YY Component
YY tensor component.
ZZ Component
ZZ tensor component.
Tensor to Vector
XY Component
XY tensor component.
YZ Component
YZ tensor component.
ZX Component
ZX tensor component.
Min Principal
Mid Principal
Max Principal
Min Deviatoric
Mid Deviatoric
Max Deviatoric
Calculated minimum principal magnitude.
Calculated mid principal magnitude.
Calculated maximum principal magnitude.
Minimum principal magnitude of the deviatoric.
Mid principal magnitude of the deviatoric.
Maximum principal magnitude of the deviatoric.
Mean von Mises
Determinant
Max Shear
Octahedral
Min Principal
Mid Principal
Max Principal
Calculated mean of the tensor.
Calculated effective stress using von Mises criterion.
Determinant of the symmetric tensor matrix.
Calculated maximum shear magnitude.
Calculated Octahedral shear stress.
Calculated minimum principal vector.
Calculated mid principal vector.
Calculated maximum principal vector.
Result Options Form
This subordinate form appears when the Result Options button is selected on the Results
Selection form.
Result Options
Current Result
Displays the current selected result.
Select Default Load Case
Lists all of the selected load cases. A default load case must be selected.
CHAPTER 13
Insight
251
12
Data Type:
Numerical Form:
Associated With:
Layer Position:
None
Scalar To Scalar
Transform Method:
Result Mapping
Element Constant
◆
Nodal Average
Element Nodal
Unknown
Unknown
Unknown
Coord Transformations
Transform
Coordinate Frame
None
If multiple layers are defined, select a desired layer position from the pull-down menu.
Select a desired transform method if the result data type does not match the tool data type.
Results associated with elements can be handled in one of three ways. Element Constant will average all the results of the specified type associated with each element to obtain a single value. This value will then be used for any subsequent operations such as obtaining nodal averaged values for fringe or isosurface display.
Nodal Average will obtain a value at the nodes by averaging the extrapolated nodal values for all of the elements associated the each node. Element Nodal will preserve multiple results at element nodes until the final display. This method will show discontinuity for element targeted fringe tools and will not average results for entities not displayed or targeted by a tool.
OK
To specify an alternate coordinate system for display of vector or tensor results, depress the
Transform toggle and enter a coordinate frame in the databox using the list format. For example,
Coord 1.
252
PART 6
Results Postprocessing
12
Isovalue Setup
The following subordinate form appears when the Isovalue Setup button is selected on the
Results Selection form.
0.0
Result Isovalue Setup
1.0
Isovalue
0.0
Ending Value
1
0.5
0.5
Number of Isos
1
1.0
5
Adjust the slidebar to set an initial value for the isosurface, or enter a value in the databox. The valid range will be automatically calculated based on the range of the current result.
If the number of isosurfaces is greater than one, adjust the slidebar to set an end value for the isosurface, or enter a value in the databox.
OK
Adjust the slidebar to set a value for the number of isosurfaces to be displayed, or enter a value in the databox. The surfaces will be evenly spaced from the starting to ending value. If only one surface is used, the starting and ending value will be equal.
CHAPTER 13
Insight
253
Isosurface Coordinate Selection
The following subordinate form appears when the Isosurface Coordinate Selection button is selected on the Insight Imaging form.
Isosurface Coordinate Selection
Existing Coordinate Frame Axes
R
-CoordinateFrame(0)
Select a coordinate frame from the list of existing frames.
Any rectangular, cylindrical, or spherical coordinate frame is valid. Frame 0 is the global system.
12
Coordinate Axis
◆
X-Axis
Y-Axis
Z-Axis
0.0
Starting Value
0.0
Ending Value
1
Number of Isos
OK
0
0
1
Cancel
1.0
1.0
5
Select an axis for the selected coordinate frame.
Adjust the slidebar to set an initial value for the isosurface, or enter a value in the databox. The valid range will be automatically calculated based on the range of the selected coordinate frame/axis for the posted groups.
If the number of isosurfaces is greater than one, adjust the slidebar to set an end value for the isosurface, or enter a value in the databox.
Adjust the slidebar to set a value for the number of isosurfaces to be displayed, or enter a value in the databox. The surfaces will be evenly spaced from the starting to ending value. If only one surface is used, the starting and ending value will be equal.
254
PART 6
Results Postprocessing
12
Tool Attributes
The following forms are accessible from the Insight Imaging form when the applicable
Attributes button is selected. Each tool type has a unique Attributes form to set the graphical display controls specific to the tool.
❏
❏
Surfaces of constant result or coordinate value.
❏
Tracing of a particle path (or paths) through a vector field.
❏
Surfaces generated along streamlines displaying a vector fields vorticity as a ribbon along streamlines.
❏
❏
Three dimensional contour surfaces through solids.
Contoured bands of color representing ranges of results value.
❏
Lines of constant result value.
Element-based polygon-fill or wireframe plot with color representing results values.
❏
Tensors are depicted at the result locations as three dimensional cubes or squares with vectors showing direct and shear components.
Vector plot of results components or resultants.
❏
❏
❏
Colored scaled symbols representing scalar results.
Annotation representing the actual result value displayed at the result locations.
❏
❏
Displays the model and posted tools in a deformed state.
Assigns a result to the mouse for screen and spreadsheet display.
CHAPTER 13
Insight
255
Isosurface Attributes
None
Free Edge
Wireframe
Shaded
Transparent
Hidden Line
Display nothing on this portion of the clipped model.
Display the clipped model as a wireframe image with inter-element boundaries visually suppressed. Shows only those edges belonging to only one element.
Display the clipped model as a wireframe image including any interelement boundaries.
Display the clipped model as a solid-shaded image.
Display the clipped model as a transparent, solid-shaded image whose degree of transparency is specified by the Model Transparency slidebar on the Insight Preferences form.
Display the clipped model as a hidden line plot by suppressing the rendering of those edges which would not normally be visible on a solid object.
Isosurface Attributes Form
Select a color for the isosurface. Mapped will map the current result or coordinate range to the spectrum for color assignment.
12
Isosurface Attributes
Isosurface Name
Isos_1
Mapped
Color:
0.0
1.0
Transparency
0
Clip at Isosurface
< Display:
> Display:
None
None
OK
A default name for the isosurface is provided.
Enter a new name, if desired.
Adjust the slidebar to set a value for the transparency for the isosurface, or enter a value in the databox. A value of 0.0 is opaque, 1.0 is completely transparent. A completely transparent isosurface is often useful as a target for other tools.
Select a display method for all of the model which is less than the start isovalue.
Select a display method for all of the model which is greater than the end isovalue.
Select this option to define the isosurface as clipping. A clipping isosurface will display the model in the specified methods on either side of the isosurface. Setting different display methods on either side of a clipping isosurface will provide greater visualization of where specified thresholds are exceeded.
256
PART 6
Results Postprocessing
12
Streamline Attributes
Select a color for the streamline. Mapped will map the current result to the spectrum for color assignment.
Streamline Attributes
Streamline Name
Streaml_1
Color:
Style:
1
Mapped
Solid
10
Stream Width
Existing Rake(s)
1
A default name for the streamline is provided. Enter a new name, if desired.
Select a streamline style from the pull-down menu.
Adjust the slidebar to set a value for the stream width multiplier, or enter a value in the databox.
Existing rakes will appear in the listbox. A rake MUST be selected for a streamline tool. If no rakes exists, create one using the Rake Specification form.
OK Cancel
Displays
CHAPTER 13
Insight
257
Streamsurface Attributes
Select a color for the streamsurface. Mapped will map the current result to the spectrum for color assignment.
Streamsurface Attributes
Streamsurface Name
Streams_1
Color:
Style:
1
Mapped
Solid
10
Stream Width
0.0
1
1.0
Transparency
0.0
0
Ribbon Scale
Existing Rake(s)
0.025
1.0
A default name for the streamsurface is provided. Enter a new name, if desired.
Select a streamsurface style from the pull-down menu.
Adjust the slidebar to set a value for the stream width multiplier, or enter a value in the databox.
Adjust the slidebar to set a value for the transparency for the streamsurface, or enter a value in the databox. A value of 0.0 is opaque, 1.0 is transparent.
Adjust the slidebar to set a value for the ribbon width as a screen fraction, or enter a value in the databox.
12
OK Cancel
Existing rakes will appear in the listbox. A rake MUST be selected for a streamsurface tool. If no rakes exists, create one using the Rake Specification form.
258
PART 6
Results Postprocessing
Threshold Attributes
12
Threshold Attributes
Threshold Name
Thresh_1
Mapped
Color:
0.0
1.0
Transparency
1
0
10
Edge Width
Edge Display
OK
1
Turns ON/OFF the edge display.
A default name for the threshold is provided. Enter a new name, if desired.
Select a color for the threshold. Mapped will map the current result range to the spectrum for color assignment.
Adjust the slidebar to set a value for the transparency for the threshold, or enter a value in the databox. A value of 0.0 is opaque and 1.0 is transparent.
Adjust the slidebar to set a value for the edge width multiplier, or enter a value in the databox. Edges are displayed where threshold surfaces intersect element edges or faces.
CHAPTER 13
Insight
259
Fringe Attributes
Turns ON/OFF the contour edge display. Contour edges are displayed at the current range thresholds.
Fringe Attributes
Fringe Name
Fringe_1
0.0 1.0
Transparency
0
1
Edge Display
10
Edge Width
1
Style:
Element Display
Solid
0.0
Continuous Tone
Shrink Factor
0
1.0
OK
A default name for the fringe is provided. Enter a new name, if desired.
Adjust the slidebar to set a value for the transparency for the fringe, or enter a value in the databox. A value of 0.0 is opaque and 1.0 is transparent.
Adjust the slidebar to set a value for the contour width multiplier, or enter a value in the databox.
Select a contour line style from the pull-down menu.
Turns ON/OFF the element edge display.
Adjust the slidebar to set a value for the shrink factor for the targeted faces for the fringe tool. A value of 0.0 is full size, 1.0 is completely collapsed to the face centroid.
12
Turns ON/OFF continuous tone fringe plots.
This feature will be disabled on display devices not supporting true color.
260
PART 6
Results Postprocessing
12
Contour Attributes
Select a color for the contour lines. Mapped will map the current result range to the spectrum for color assignment.
Contour Attributes
Contour Name
Contour_1
Color:
Style:
0
Mapped
Solid
50
Label Frequency
20
1 10
Contour Width
1
OK
A default name for the contour is provided. Enter a new name, if desired.
Select a contour line style from the pull-down menu.
Adjust the slidebar to set a value for the label frequency, or enter a value in the databox. A value of zero will display no spectrum level labels and a non-zero value will display labels along the contour lines.
Adjust the slidebar to set a value for the contour width multiplier or enter a value in the databox.
Element Attributes
Select a color for the elements. Mapped will map the current result range to the spectrum for color assignment.
Element Attributes
Element Name
Element_1
Mapped
Color:
0.0 1.0
Shrink Factor
0
Element Fill
OK
A default name for the element is provided. Enter a new name, if desired.
Adjust the slidebar to set a value for the shrink factor for the element attributes for the tool, or enter a value in the databox. A value of 0.0 is full size and 1.0 is completely collapsed to the element centroid.
Turns ON/OFF the element face fill. Color coded elements will either be displayed as shaded faces or wireframe edges.
CHAPTER 13
Insight
261
Tensor Attributes
A default name for the tensor is provided. Enter a new name, if desired.
Select a color for the tensor box and the tensor vectors.
Mapped will map the current result range to the spectrum for color assignment.
Tensor Attributes
Tensor Name
Tensor_1
Tensor Box Attributes
Color:
Tensor Scale:
0.01
Mapped
Values
1.0
Tensor Vector Attributes
Color:
Vector Scale:
0.01
Mapped
Values
1.0
Scale Factor
0.025
Tensor Box Display
Tensor Box Fill
Tensor Display:
Principals
Scale Factor
1
0.025
Vector Width
1
Direct Vector Display
Shear Vector Display
Vector Fill
10
Turns ON/OFF the polygon fill of the tensor box faces.
Turns ON/OFF the display of the tensor box.
Select a scaling method for the tensor box and vectors. Values will vary the size based on the result magnitude. Screen will use a fixed scale based on the screen size.
Adjust the slidebar to set a scale factor for the tensor box and vectors, or enter a value in the databox. This will be a screen size multiplier.
Adjust the slidebar to set a vector width multiplier, or enter a value in the databox.
Turns ON/OFF the display of the direct vectors.
OK
Turns ON/OFF the display of the shear vectors.
Turns ON/OFF the display of polygon filled vector arrowheads.
Select a display method for the tensor orientation from the pull-down menu. Principals will orient the tensor in the direction of principal stress. Components will orient the tensor in the coordinate system defined for the result.
12
262
PART 6
Results Postprocessing
12
Vector Attributes
Select a scaling method for the vectors. Values will vary the size based on the result magnitude.
Screen will use a fixed scale based on the screen size.
Vector Attributes
Vector Name
Vector_1
Color:
Vector End:
Vector Scale:
Vector Display:
Resultant
0.01
Mapped
Head
Values
1.0
Scale Factor
1
0.1
10
Vector Width
1
Double Head
Vector Fill
Reflection
Tail Display
OK
A default name for the vector is provided. Enter a new name, if desired.
Select a color for the vectors. Mapped will map the current result range to the spectrum for color assignment.
Select a vector end registration method. Head will connect the vector head to the result location. Tail will register to the tail.
Adjust the slidebar to set a scale factor value for the vectors, or enter a value in the databox. This will be a screen size multiplier.
Adjust the slidebar to set a vector width multiplier, or enter a value in the databox.
Turns ON/OFF the display of double headed vectors.
Turns ON/OFF the display of polygon filled vector arrowheads.
Turns ON/OFF the display of reflected
(two way) vectors.
Turns ON/OFF the display of vector tails.
Select a display method for the vectors. Resultant will display the resultant vector. Components will display the individual vector components oriented in the coordinate system defined for the result.
Marker Attributes
Select a color for the markers. Mapped will map the current result range to the spectrum for color assignment.
Marker Attributes
Marker Name
Marker_1
Color:
Type:
Scale:
0.005
Mapped
Triangle
Values
1.0
Scale Factor
0.015
OK
A default name for the marker is provided. Enter a new name, if desired.
Select a marker icon type style. These icons will be positioned at the element centroids or nodal locations.
Adjust the slidebar to set a scale factor value for the markers, or enter a value in the databox. This will be a screen size multiplier.
Select a scaling method for the marker icons. Values will vary the size based on the result magnitude. Screen will use a fixed scale based on the screen size.
Value Attributes
Value Attributes
Value Name
Value_1
Color:
Format:
Mapped
E-Component
OK
A default name for the value is provided. Enter a new name, if desired.
Select a color for the values. Mapped will map the current result range to the spectrum for color assignment.
Select a format for displaying the values. “E” will use exponential format (i.e.,
1.0E+04). “F” will use fixed format (i.e., 1000.0). “G” will use either “E” or “F” depending on the value magnitude. “I” will use an integer format (i.e., 1000).
CHAPTER 13
Insight
263
12
264
PART 6
Results Postprocessing
12
Deformation Attributes
Select a scaling method for the deformation. Screen will scale the deformation based on the current screen size. True will show the actual deformation multiplied by the scale factor.
Deformation Attributes
Deform Name
Deform_1
Scale:
0.0
Screen
1.0
Scale Factor
0.1
Undeformed Model
Color:
Blue
Style:
Free Edge
A default name for the deform is provided. Enter a new name, if desired.
Adjust the slidebar to set a scale factor for the deformation, or enter a value in the databox. If the method is Screen, the scale factor will be multiplied by the screen size. If the method is True, the scale factor will be used as a true scale multiplier of the actual deformation. True scale should be used to display transient animations. The slidebar extremes will expand if a value exceeding the current range is entered in the databox.
OK
Turns ON/OFF the display of the undeformed model. The color and style of the undeformed model can be controlled with the Color and Style menus.
Cursor Attributes
Cursor Attributes
Cursor Name
Cursor_1
Color:
Red
Format:
E-Exponent
Cursor Display:
Values
Display Values On Form
OK
A default name for the value is provided. Enter a new name, if desired.
Select a color for the values.
Select a format for displaying the values. “E” will use exponential format (i.e., 1.0E+04). “F” will use fixed format (i.e., 1000.0). “G” will use either “E” or “F” depending on the value magnitude. “I” will use an integer format (i.e., 1000).
Toggle this button to control if the cursor tool information is to be added to the spreadsheet as displayed on the screen.
Select the cursor tool to display either the result values or the node/element
IDs. Both the IDs and result values will be displayed on the spreadsheet.
CHAPTER 13
Insight
265
Insight Control
The Insight Control capabilities are found in the Insight Control pull-down menu on the
MSC.Patran main form. There are five control forms which are listed:
❏
❏
❏
❏
❏
❏
❏
Post/Unpost Tools
The following form appears when the Post/Unpost Tools option is selected in the Insight
Control pull-down menu.
Post/Unpost Tools
Existing Tools
IS-Isos_1:Stress,vonMises
FR-Fringe_1:Displacement
Lists existing tools. The tools that are posted are selected (highlighted) in the listbox.
12
Unselect All
OK
266
PART 6
Results Postprocessing
12
Named Postings
The following subordinate form appears when the Named Postings Options button is selected on the Post/Unpost Tools form.
Posts the selected Named Postings. Only the tools defined by the selected postings will be posted. All other tools will be unposted.
Named Postings
Named Postings
Lists existing named postings. Select a posting from the listbox to Post, Delete, Obtain Information, or
Rename.
Post Selected
Create...
Info...
Rename...
Delete
Cancel
Renames the selected Named Posting.
Deletes the selected Named Posting. This will not delete the tools.
Displays a list of the tools defined by the selected
Named Posting.
Creates a Named Posting. The currently posted tools will be assigned to the name provided.
CHAPTER 13
Insight
267
Isosurface Control
The following form appears when the Isosurface Control option is selected in the Insight Control pull-down menu.
The result/coordinate associated with the selected isosurface will be displayed here as information.
Isosurface Control
Isosurface to Control
Lists all posted isosurfaces. Select an isosurface from the list to activate it for dynamic control using this form.
12
Isosurface Result
The form actions may be switched to be either interactive or user controlled. Immediate mode will allow for display updates as the values are being changed. Upon Apply will update the display only when you press the apply button.
Form Actions
Immediate
Upon Apply
0.0
Isovalue
0.0
Ending Value
0.5
Apply
0.5
Cancel
1.0
1.0
Adjust the slidebar to set a value, or enter a value in the databox, for single surface isosurfaces, or a starting value for multiple surface isosurfaces. The number of displayed surfaces for an isosurface tool is modified
(p. 252) (accessed through the
Results Selection form,) or by accessing
(p. 253) for coordinate driven
isosurfaces. The valid range for the values entered is determined by the current result or coordinate range.
Adjusting the slidebar or entering a value in the databox will update the display in immediate mode. The frequency of the immediate mode display update is controlled from the
Use the slidebar to set a value for the ending value for multiple surface isosurface tools or enter an ending value in the databox. This value will be tied to the isovalue for single surface tools.
268
PART 6
Results Postprocessing
12
Range Control
The following form appears when the Range Control option is selected in the Insight Control pull-down menu.
May be switched to be either interactive or user controlled. Immediate mode will allow for display updates as the values are being changed. Upon Apply will update the display only when the apply button is pressed.
Select Tool for Active Range
Range Control
Select a tool from this list to display or modify its spectrum and range values. This tool will be associated with the displayed spectrum.
Form Actions
Immediate
Upon Apply
Active Range Method
Auto
Viewport
Default Range Method
Auto
Selected Tool
Viewport
0.0
Freeze Range Values
1.0
Min.
0.0
Max.
1
0
1
1.0
12
Levels
12
Used to hold the current minimum and maximum values for the active
Auto range. If the values are not frozen, they will be set automatically based on the active range tool result.
If the Active Range Method is
Auto, adjust the slidebars to set a value, or enter a value in the appropriate databox, for the minimum and maximum range, and the number of levels for the active tool range.
Apply Cancel
Select a method for assigning color to the active range tool. Auto will assign color and display the spectrum ranges based on values automatically determined by the tools result. Viewport will assign color and display the spectrum ranges as those currently assigned to the Insight viewport.
Select a method for assigning color to all other tools posted. Auto will assign color based on each tools result/coordinate range. The assigned color will most likely NOT correspond to the displayed spectrum and range values, but will give a good qualitative indication of the tools’ result variations. Selected Tool will guarantee a one-to-one correspondence of assigned color to the displayed spectrum and ranges. However, it may not provide any color variation for tools other than the active range tool. Viewport will assign color levels based on the current range assigned to the Insight viewport, regardless of the Active
Range method.
CHAPTER 13
Insight
269
Animation Control
The following form appears when the Animation Control option is selected in the Insight
Control pull-down menu.
Pause/Stop or Restarts the animation currently running. The animation must be paused to enable any capability other than the start and end frame values.
If an animation is not currently defined, click this button to display
(p. 270) to first define an animation.
Animation Control
Clear...
Clears the current animation. If an animation is currently running, it may be necessary to first Pause the animation.
Pause/Stop Animation
Animation Method
◆
Cycle
Bounce
1
Step
7
Select a method for displaying the current animation.
Cycle will display the animation frames 1:n, 1:n,... Bounce will display the frames 1:n:1:n...
If an animation is currently paused, click this button to step through the animation frame-by-frame using the current method.
Start Frame
2
1
8
Adjust the slidebar to set a value, or enter a value in the appropriate databox, for the Start Frame and End Frame of the animation currently running. Changing these values will skip the display of all the frames above or below the entered values, respectively.
End Frame
1
8
8
Current Frame
8
Adjust the slidebar or enter a value for the current frame to display a paused animation. Adjusting the slidebar or accordingly.
Animation Speed
Reduced Rendering
OK
Adjust the slidebar to control the speed of the animation.
Having the slidebar set fully to Fast will animate as quickly as the graphics device is able.
12
Toggle the reduced rendering mode for animations. The reduced rendering mode will display only the wireframe to speed up animation on non-3D devices.
270
PART 6
Results Postprocessing
12
Animation Setup
The following subordinate form appears when the Setup button is selected on the Animation
Control form. Use this form to create an animation sequence.
There are two basic methods of animation, 2D and 3D. 2D animations will be faster on display devices without hardware accelerators and with large models. View manipulations are not supported during 2D animations. 3D animations might be slower but do support rotations, panning and zooming during an animation. The animation of tools will automatically generate frames using the animation attributes defined for each tool. All posted tools will be displayed, but only tools with animation enabled will change from frame to frame. Each tool with animation enabled will have its results interpolated (linear interpolation only) to each animation frame based on the attributes specified for the tool on the Animation Attributes form.
If a tool’s animation method is Global Variable, each animation frame result will be interpolated based on the available results associated with global variables bracketing the current animation frame. This method is only available for tools associated with multiple loadcases. For example, if a tool is to be animated using six result load cases with time ranging from zero to two seconds, and the number of frames is set to eleven, results will be linearly interpolated from the existing data at Time=0.0, 0.2, 0.4,..., 2.0. If a desirable global variable does not exist for the selected results for a tool, the default LOAD CASE INDEX variable may be used. LOAD CASE INDEX assigns an incremental integer count to each selected load case and uses it to interpolate animation frames as with any other global variable.
The Ramp and Sinusoid animation methods will scale the static default result for each enabled tool using a ramp or sinusoid scale factor which is determined for each frame. These methods will scale the current starting isovalue for animation of coordinate driven isosurfaces.
The 2D animations provide additional support for the generation and retrieval of image files.
These files can either be generated automatically during an animation of tools or created individually to be played back later. The creation of individual animation frames enables the user to form arbitrary animations. The image files are handled using their version numbers to determine which frame they define.
Caution should be used in animating multiple tools with multiple methods pointing to multiple results simultaneously. The resultant display will be difficult to interpret.
Animation Setup
Animation Mode:
Animate Tools - 2D
Animation Tool(s)
The animation modes are Animate Tools - 3D,
Animate Tools - 2D, Animate Images - 2D, and Create
Images-2D. The 3D animations may be slower on some devices but allow view manipulations during animations. The 2D animation capabilities also provide for the optional storage and retrieval of animation frame images. The Create Images mode will capture the current display and create a file for future redisplay.
Non-Animation Tool(s)
All the posted tools will be listed in these two listboxes. Tools with animation enabled will be listed in the upper listbox and those with animation disabled will be listed in the lower listbox. Only the tools listed in the upper listbox will animate although all tools will
be displayed during an animation. Select a tool in either listbox to display the applicable
(p. 249) form. The listboxes will be
updated depending on the Enable Animation toggle value on the Animation Attributes form. These listboxes are not used when animating images.
2
Frames
8
Save Frame to Files
Image File Definition insight.img.*
Image File Definition...
Animate
60
Cancel
2D animations can optionally be stored or retrieved from image files. The image files must all have the same filename with the version numbers consecutive from .01.
The Animate/Create Image File button will either initiate the create of an animation or create an image file if the mode is Create Images.
Adjust the slidebar to set a value, or enter a value in the databox, for the number of animation frames to be created. This value is used for the redisplay frame number when creating an image file.
CHAPTER 13
Insight
271
12
272
PART 6
Results Postprocessing
12
Modal Animation
Provides rapid access to a modal animation display. The animation is initiated when the
Animate button is pressed. The Cancel button will terminate the animation. The Animation
Control form can be displayed to provide further control of the running animation if desired.
Modal Animation
Current Load Case(s)
Current Result
If results have been selected for a modal animation, they will be displayed here.
Results Selection...
Animation Method
◆
2D Mode
3D Mode
Animate
Cancel
Displays the
Select either 2D or 3D Mode for animation. 2D is often faster, 3D allows for view manipulation during an animation.
Initiates a modal animation.
Rake Specification
The following form appears when the Rake Specification option is selected in the Insight Control pull-down menu.
Rake Specification
Rake Name
Enter a name for a new or existing rake.
Existing Rake(s)
Lists all existing rakes. Select a rake name from the list to modify or delete.
Primary Nodes
Apply
Cancel
Delete
Enter a list of primary nodes for streamsurfaces. This release of MSC.Patran does not provide screen picks for node selection.
Deletes the selected rake. A rake may not be deleted if it is currently referred to by a stream tool.
CHAPTER 13
Insight
273
Cursor Results
The following form is displayed automatically when a cursor tool is posted or by selecting the
Cursor Results option from the Insight Control menu.
Cursor Results
Cursor Tool Summary
Cursor Tool: Cursor_1
Result: 4.1-Stress Invariants
Load Case: STATIC LOAD AT END
Entity: Node Scalar
Min: -1461.81 @ ID= 265
Max: 6183.2 @ ID= 427
ID List
Node
Information regarding the current posted cursor tool will be displayed here.
ID
Node 10
Node 25
Node 34
Value
200.230407715
165.079574585
122.703704834
Enter a node or element list depending on where the cursor tool is targeted. The IDs specified will be added to the spreadsheet and the values will be displayed on the screen.
Note:
Be aware that adding large numbers of entries to a spreadsheet is very time consuming and not recommended.
12
Node ID = 25, ACID = 0
Location = -2. 7.177 -0.1414
Cascade Spread Sheet
Reset Cancel
Selecting a cell in the spreadsheet will provide additional information in the textbox.
Allows screen selected entities to either overwrite the last spreadsheet row or add a new one. Entering a list of multiple entities in the databox will automatically toggle the spreadsheet to cascade.
274
PART 6
Results Postprocessing
12
Cursor Results to File
The following form is displayed from the Cursor Results spreadsheet form.
Set this switch to either append, overwrite or preview the specified file. The preview option will write the text to the system window.
Cursor Results to File
Filter
/okinawa/users/smith/*.rep
File Options
◆
Overwrite
Append
Directories
/smith/.
/smith/..
/smith/.fminit2.0
/smith/Exercises
/smith/Mail
/smith/Part_2_basic_functions
/smith/Part_4_FEM
File List
[ ]
Preview
Displays
Displays
Cursor Results File Name patran.rep
- Apply -
Filter Cancel
CHAPTER 13
Insight
275
Cursor Results File Format
The following form is displayed from the Insight Cursor Results File Form. This form provides control of the file formatting for output of the information currently in the cursor tool spreadsheet.
The page, width, lines and margin databoxes are used to control the page numbering and page sizing.
Page No.
1
Cursor Results File Format
File Width
72
Select Columns to Output
1- ID
2- ACID
3- X Coord
4- Y Coord
5- Z Coord
6- Value
Lines/Page
52
Left Margin
8
Column Labels/Formats
Header
1
ID
2
ACID
3
4
X Coord
Y Coord
Input Labels/Formats
The text for the column headings and the formats for the columns are defined by the cells in the format spreadsheet. The column formats are viewed by sliding the horizontal scroll bar. Entries are edited by selecting a cell and modifying the text as it appears in the databox. The format strings are described in the
text_write_string
(p. 112) in the
PCL and Customization.
Text Title/Header/Footer Format
Title Text Format
MSC.Patran Release 1.1-X293 01/14/93 03:33:0>
MSC.Nastran Results
Load Case: STATIC LOAD AT END
1
Input Title/Header/Footer Format
Up to 5 lines of text are available to be defined for the file title and page headers and footers.
Entries may be edited by selecting the spreadsheet cell and modifying the text as it appears in the databox.
12
OK
Access the lines of text to be used for the title (appears once at the top of the file), the header (appears at the top of each page) and the footer (appears at the bottom of each page). If the format string %I% appears in the header or footer, the current page number will be inserted in its place.
Select any number of items from the available list to be included as columns in the output file.
276
PART 6
Results Postprocessing
12
Cursor Results File Sorting
The following form is displayed from the Cursor Results File Form. It controls the output columns and methods for sorting of the spreadsheet data for file output.
Output File Sort Method
Sort Method
◆
Unsorted
Ascending
Descending
Select a method of sorting. Unsorted will print the spreadsheet rows in the order they appear.
Ascending or Descending will sort the spreadsheet rows for output based on the values of the selected column.
Sort Basis
◆
Algebraic Value
Absolute Value
Column to Sort
1- ID
2- ACID
3- X Coord
4- Y Coord
5- Z Coord
6- Value
The sorting can be either on the basis of the
Algebraic (actual) or Absolute value.
If the output is to be sorted a column must be selected from the listbox.
OK
Global Settings
The global settings are controlled through two forms. The
controls the colors used in the current spectrum. The
the default graphics such as model rendering style, color, entity labeling, and others.
CHAPTER 13
Insight
277
Insight Spectrum
The following form is displayed when the Spectrum option is selected in the Display menu.
Insight Spectrum
Spectrum Type
◆
Default
Standard
Temperature
Rainbow
Hue
Hue Scale
Gray Scale red Scale
Alt. Spectrum 1
Alt. Spectrum 2
Select a spectrum type to assign to the Insight viewport. Each spectrum has a maximum of twelve color levels. Any spectrum setting other than the default will effect the colors of shaded entities
(faces).
Apply Cancel
12
Insight Preferences
The Insight Preferences form provides capabilities for control settings which are specific to the
Insight application but have global effects on its function. The Display Method pull-down menu controls the method of displaying the finite element model in the Insight viewport. Posting a
Fringe tool to the model faces or a clipping isosurface will take precedent over the default methods.
Free Edge
Wireframe
Shaded
Transparent
Hidden Line
Display the model as a wireframe image with inter-element boundaries visually suppressed. Shows only those edges belonging to only one element.
Display the model as a wireframe image including any inter-element boundaries present in the posted group.
Display the model as a solid-shaded image.
Display the model as a transparent, solid-shaded image whose degree of transparency is specified by the Model Transparency slidebar.
Display the model as a hidden line plot by suppressing the rendering of edges not normally visible on a solid object.
278
PART 6
Results Postprocessing
12
Insight Preferences Form
Set a value for the default model face transparency. A value of 0.0 is opaque and 1.0 is transparent. Control face and edge colors.
Displays the element edges on faces.
Select a display method from this pull-down menu for the default model rendering style.
Default Model Display
Display Method
Free Edge
Edge Display
0.0
Insight Preferences
Reduced Rendering
All Displays
1.0
Animation
Isosurface Control
Range Control
Model Transparency
Background Color
Black
Edge Color
White
Face Color
White
1%
Label Display
Node Labels
Element Labels
CoordSys Labels
Slider Resolution
Free Edge Display
◆
Feature Angle
Element Association
0 30
Shading/Lighting:
Gouraud/Dynamic
Auto Find
Apply
Feature Angle
Cancel
25%
90
Controls the display of faces using either Flat, Gouraud, or No shading and use either static or dynamic lighting of shaded faces. With dynamic lighting, the shading is modified as the model is rotated. Auto Find controls the automatic fit performed after view rotations.
Select any of these options on to have all filled polygons drawn as wireframe outlines during the specified operation(s). This will increase the graphics speed when hardware shading is not available.
Select a color for the display background. Fancy is only available for true color devices.
Adjust the slidebar to define the percentage change between updates for all non-integer dynamic slidebars used in the Insight application forms.
The free edges of a model can be determined either by the angles between adjacent faces
(Feature Angle) or by displaying only edges belonging to one element
(Element Association). The slidebar is used to set the angle used for the feature angle method. All edges with an angle greater than the feature angle between normal will be displayed.
Control the display of Node, Element, and Coordinate labels. Element labels will only be displayed when elements are displayed by setting the model display method to
Wireframe, or by posting an element tool.
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
14
Numerical Methods
■
■
Result Case(s) and Definitions
■
■
■
■
280
PART 6
Results Postprocessing
13
14.1
Introduction
A result in MSC.Patran is an array of one, three, or six numbers that represent a physical results quantity associated with finite element entities. These results are computed by the analysis program and loaded into or referenced by the MSC.Patran database by an application interface which translates the results.
Results can be retrieved only after the following questions are resolved:
•
What Result Case does it belong to? See
Result Case(s) and Definitions
•
Are the results a scalar, vector, or tensor quantity? See
•
In what coordinate system do the results belong? See
•
Are the results associated with nodes or elements? See
•
Are the results complex or single valued? See
•
What layer or position do the results belong to? See
•
For element results, where in the element are they computed? See
Each question involves an attribute which characterizes the result and differentiates it from other results. Every result must have all of these attributes defined before it can be retrieved from the database. This chapter dedicates itself to explaining these attributes and the internal workings of the program when these attributes are modified and manipulated.
CHAPTER 14
Numerical Methods
281
14.2
Result Case(s) and Definitions
Results for each model are partitioned into identifiable sets called Result Cases. A Result Case may correspond to a static load case, a load step in a nonlinear analysis, a mode shape in a normal mode analysis, or a myriad of other analysis types. Result Cases generally correspond to
Load Cases from an analysis run as defined and set up in MSC.Patran. The terminology between
Load Case and Result Case is interchangeable in many cases. However it is possible in
MSC.Patran to import results that are not associated to a Load Case. For this reason result sets are referred to as Result Cases as opposed to Load Cases.
Each item in the listbox filled with result sets corresponds to only one Result Case. Each Result
Case is associated with one or more global variables. Global variable are results that are global to a particular set of result and not each individual finite element entity. All results have at least one global variable, that being the LOAD CASE INDEX. This is basically an internal ID of the
Result Case. Other global variables can include mode number, frequency, time, and design cycles/variables. The global variables can be used:
•
to select Result Cases for filter display in the listbox
•
as variables in graph (XY) plots
•
as animation start and end values (transient)
•
in text reports
The MSC.Patran result postprocessor treats all Result Cases on an equal basis. There is no distinction between a static, nonlinear analysis, transient, or modal analysis except as indicated in its title. A result type can exist in one or more Result Cases. Once a group of Result Cases are selected, the associated result types are retrieved from the database. Duplicate and conjugate (for complex results) result types are removed. The result type labels are listed in the Result listboxes.
An item in a result listbox may represent one or more result types in the database.
The MSC.Patran results postprocessor has no pre-defined result types. The tool attaches no internal significance to the labels of the result types. Result processing is completely based on the result attributes. The external translators that import results determine which labels to assign to which results from the analysis program output. Once translated and stored in the
MSC.Patran database, the source of these results are transparent to the results postprocessor.
The MSC.Patran results postprocessor allows for selection of multiple Result Cases for processing. This functionality is important for animation, xy plots, load case combination, and finding the maximum/minimum of results across load cases. More information about result data types is presented below,
Data Types.
Results may be scalar, vector, or tensor quantities. The data type of each result is determined and set by the result translator.
Scalar results have no coordinate system attributes, but vector and tensor results are always associated with some coordinate system. A tensor is defined as a symmetric matrix of rank 2 which is stored as six associated values (xx, yy, zz, xy, yz, zx). Unless otherwise noted, vectors and tensors always denote the components that represent them in a certain coordinate system. See
13
282
PART 6
Results Postprocessing
13
The plot types are associated with the data type and the associativity of the results as follows:
Scalar
Vector
Data Type
Tensor
Associativity
Node
Element
Node
Element
Node
Element
Available Plot Types
Fringe, Graph, Report, Animation, Combine &
Derive Results (Scalar Marker, Value, Isosurface,
Threshold, Contour, Element, Value & Cursor in the Insight application)
Deformation, Vector, Report, Animation, Combine
& Derive Results (Streamline & Streamsurface in the Insight application)
Report, Tensor, Animation, Combine & Derive
Results
The data type of the results can be changed to make its associated plot type available for plots.
This change may involve a derivation and/or coordinate system definition. See
From
Scalar
Vector
Tensor
To
Vector
Tensor
Scalar
Tensor
Scalar
Vector
Coordinate
System
Yes
Yes
Yes/No
Yes
Yes/No
Yes
Remark
Scalar value inserted into the specified component. Other components = 0.
Same as Scalar to Vector above.
The data system is the system as defined in the database. You can specify the output system.
Only vector components need coordinate systems.
The data system is the system as defined in the database. You can specify the output system for the tensor. A vector component can be inserted into a tensor component.
Coordinate system is required if the scalar is one component of the tensor. Principal values are invariant with respect to coordinate systems.
Only tensor components need coordinate system.
The data system is the system as defined in the database. You can specify the output system for the vector. A tensor can be reduced to its principals in vector form.
Associativity.
Results are associated with either nodes or elements, but not both. This associativity characterizes the result type. If a particular result exists both as a nodal result and an element result (e.g., energy), the result translator must create two result types with distinct result labels.
CHAPTER 14
Numerical Methods
283
You cannot change this associativity and, once defined, the attribute along with the data type determines the available plot types. Some plot types only deal with a particular associativity
(e.g., deformed plot only for nodal vector results, tensor plot only for element tensor results) but other plot types deal with both (e.g., fringe plot, xy plot, report). Some processing methods are only applicable to either nodes or elements, whereas other methods are applicable to both.
If a processing method involves elements, but results are associated with nodes, the results at these nodes will be assigned to the elements sharing the common nodes. Interpolation functions are then used to compute results at any point within the element from the results at element nodes. See
The converse is also true. If a processing method involves nodes, but results are associated with elements, the results within the elements will be extrapolated out to the nodes. See
(p. 299). To report results at the nodes from elemental data, the contribution at a
node from each surrounding element is averaged to a single scalar value (or vector or tensor depending on the data type). When derived results are requested from vector or tensor data, the order in which averaging and derivation are done is important. Control of this order is given to the user which can give different answers.
Numerical Form.
The MSC.Patran Results Processor can process complex results. Each result type has an attribute to indicate its numerical form:
Primary
Numerical Form
Real
Imaginary
Magnitude
Phase (radians)
Associated
Numerical Form
Imaginary
Other
Real
Other
Phase (radians)
Other
Magnitude
Other
Considered As
Complex
Single
Complex
Single
Complex
Single
Complex
Single
If results are complex, the option to display the values as real, imaginary, magnitude, or phase are computed (in temporal space) at a particular phase angle.
13
Real * cos
θ
+
Imaginary * sin or
Magnitude * cos
(
Phase
)
* cos + Magnitude * sin
( )
* sin where results.
θ
= 0 corresponds to purely real results and
θ
= 90
°
corresponds to purely imaginary
Magnitude and phase of complex results are computed from real and imaginary result pairs as
284
PART 6
Results Postprocessing
13
P
hase
= tan
–
1 imaginary
Magnitude
= real
∗ real + imaginary
∗ imaginary which is then converted to range
[
0 2
π ]
.
Except for the numerical form, conjugate results must have the same attributes as those of their paired results. They must belong to the same Result Case, same data type, same associativity, same layer-position, same nodes/elements, and for element results, computed at the same output location within elements.
Once converted to single form (i.e., real, imaginary, magnitude, phase angle or at a particular phase angle), results are treated the same way as non-complex results.
Layer-Position.
For plate or shell elements, results can be computed at a particular location through the thickness. For composite elements, results can be computed for a particular layer, and/or at a particular location in the thickness of a layer. These two through-thickness positions are collapsed into an attribute called layer position. Each layer position specifies a unique layer
ID (0 for homogeneous elements) and a unique location within the layer (labelled NON-
LAYERED for solids). The labels for layer positions created by the results translators indicate the actual location of the output points.
For homogeneous beams or bars, each layer position corresponds to an output location in the beam section. The layer position attributes contain the actual physical coordinates of the output points. All other layer position coordinates are dimensionless parametric coordinates. For layered beams/bars, the results are treated like plates and shells. The labels for layer positions in beams indicate the actual locations of the output points.
For homogeneous beams or bars, a dummy layer-position is created so that it has a layer position
ID for access. Composite solids are treated as composite plates/shells.
The MSC.Patran Results Postprocessor only uses the ID of the layer position to retrieve its associated results. The labels for layer position are transparent to the processor.
Target Nodes and Elements.
Each result in MSC.Patran has to be associated with a node or an element ID. A result that is associated with the whole result case is called a global variable, such as time or frequency. Results can be displayed only if their associated nodes/elements exist in the targeted entities for any given plot type. A variety of options exist to specify at which entities to target result plots:
•
ID list (i.e., list of nodes and element IDs).
•
Range for result values. This filter is based on result values from the database.
•
Lists of material properties (element results).
•
Lists of element properties.
•
Lists of element types.
•
Lists that are based on material properties.
•
Lists that are based on element properties.
•
Lists that are based on element types.
•
Lists of points that lie along an arbitrary path
CHAPTER 14
Numerical Methods
285
Results in the database can belong to a superset or subset of these ID lists, but only the results that belong to the elements/nodes effected by the intersection of these lists are able to be displayed.
Element Position.
Element results can be computed at any point in the element. The location of the output point is part of an attribute called element position. The element position contains, among other things, the parametric coordinates of the output. The result translators create these attributes and assigns them to the element results. It makes no difference to the MSC.Patran
Results Processor if this point is one of the element nodes, the element faces, the element edges, the Gaussian quadrature points, or the element centroid. The coordinate system type depends on the element topology.
Topology
Bar/Beams
Tria
Quad
Tet
Wedge
Hex
Coordinate
System Type
Parametric
Area
Parametric
Volume
Area/Parametric
Parametric
Coordinates
s
1 s
1
, s
2
, s
3 s
1
, s
2 s
1
, s
2
, s
3
, s
4 s
1
,s
2
,s
3
,s
4 s
1
,s
2
,s
3
It is important to note that:
1. All coordinates are in range [0..1].
2. For wedges, s
1
, s
2
, s
3
= area coordinates, s
4
= parametric coordinates.
13
286
PART 6
Results Postprocessing
13
14.3
Derivations
The following table provides additional definitions for the selected result derivations. These include tensor to vector, tensor to scalar, and vector to scalar resolutions.
Transform Type
Derivation
Method
None Scalar to Scalar
Vector to Vector
Tensor to Tensor
Vector to Scalar
Magnitude
Description
No transformation is used if the result data type matches the plot tool’s data type.
Vector magnitude.
X Component
Y Component
1st vector component.
2nd vector component.
Z Component
3rd vector component.
Tensor to Scalar XX Component
XX tensor component.
YY Component
YY tensor component.
ZZ Component
ZZ tensor component.
XY Component
XY tensor component.
YZ Component
YZ tensor component.
ZX Component
Min Principal
ZX tensor component.
Calculated minimum principal magnitude.
Mid Principal
Max Principal
1st Invariant
2nd Invariant
3rd Invariant
Hydrostatic von Mises
Tresca
Max Shear
Octahedral
Calculated middle principal magnitude.
Calculated maximum principal magnitude.
Calculated 1st invariant
Calculated 2nd invariant
Calculated 3rd invariant
Calculated mean of the three normal tensor components.
Calculated effective stress using von Mises criterion.
Calculated Tresca shear stress.
Calculated maximum shear magnitude.
Calculated Octahedral shear stress.
Tensor to Vector Min Principal
Mid Principal
Max Principal
Calculated minimum principal vector.
Calculated middle principal vector.
Calculated maximum principal vector.
CHAPTER 14
Numerical Methods
287
Below are the equations and examples of the derivation methods:
Important:
These equations for calculating invariants are not recommended for complex results since phase is not taken into account.
von Mises Stress.
von Mises stress is calculated from the following equation:
σ′
=
( σ
–
σ )
2
+
( σ
–
2
σ )
2
+
( σ
–
σ )
2
)
+ 3
( τ
2
x y
+
τ
2
y z
+
τ
2
zx
)
Example: The elements shown below have the following stress contributions:
N19 N20 N21
E9
E10
13
N10
E1
N11
E2
N12
N1
1
Elem. ID
2
9
Node ID
11
10
11
20
19
1
2
11
10
2
3
12
88.67
57.42
59.37
44.32
67.37
4.72
17.99
σ
x
46.2
93.39
68.37
44.32
93.39
N2
0.00
0.00
0.00
0.00
0.00
0.00
0.00
σ
z
0.00
0.00
0.00
0.00
0.00
24.41
5.44
10.16
10.40
11.16
8.15
7.68
σ
y
13.01
25.33
12.16
10.40
25.33
N3
0.00
0.00
0.00
0.00
0.00
0.00
0.00
τ
y z
0.00
0.00
0.00
0.00
0.00
23.95
-34.02
-20.73
-1.01
-18.73
-15.28
-4.61
τ
x y
5.13
17.45
-19.73
-1.01
17.45
0.00
0.00
0.00
0.00
0.00
0.00
0.00
τ
z x
0.00
0.00
0.00
0.00
0.00
288
PART 6
Results Postprocessing
13
Elem. ID
10
Node ID
11
12
21
20
σ
x
100.37
14.16
57.42
-5.63
4.72
σ
5.44
5.72
8.15
y
σ
z
0.00
0.00
0.00
0.00
τ
x y
-30.73
-34.02
-22.03
-15.28
τ
y z
0.00
0.00
0.00
0.00
τ
0.00
0.00
0.00
0.00
z x
The von Mises stress calculated at node 11 when nodal averaging is done first due to the contribution from each element is 78.96. When the von Mises derivation is done first and then averaging at the nodes takes place, the calculated von Mises stress is 79.02. Thus a difference can arise depending on whether the averaging is done first or the derivation. This can be true for all derived results.
Node 11
σ
x
σ
y
E1
E2
E9
E10
Average
68.37
59.37
67.37
100.37
73.87
Average then Derive
Derive then Average
12.16
10.16
11.16
14.16
11.91
σ
0.00
0.00
0.00
0.00
0.00
z
τ
x y
-19.73
-20.73
-18.73
-30.73
-22.48
τ
y z
0.0
0.00
0.00
0.00
0.00
τ
z x
0.0
0.00
0.00
0.00
0.00
von Mises
Stress
71.82
65.68
70.45
108.10
79.02
78.96
79.02
Important:
It must be noted also that for von Mises and other derived results, the calculations are generally valid only for stresses. Although these operations can be performed for any valid tensor or vector data stored in the database, quantities such as tensor strains are not appropriate for von Mises calculations. To calculate a true von
Mises strain the strain tensor must be converted to engineering strains by multiplying the shear components by a factor of two.
Octahedral Shear Stress.
Octahedral shear stress is calculated from the following equation:
τ
o c t
=
( σ
–
σ )
2
+
( σ
–
σ )
2
+
( σ
3
–
σ )
2
)
+
6
( τ
2
x y
+
τ
2
y z
+
τ
2
zx
)
CHAPTER 14
Numerical Methods
289
From the von Mises example above the octahedral shear stress is:
Octahedral Shear Stress
Average/Derive
Derive/Average
Node 11
37.22
37.25
Hydrostatic Stress.
Hydrostatic stress is calculated from the following equation:
σ
=
σ
+
σ
3
y
+
σ
z
From the von Mises example above the hydrostatic stress is:
Hydrostatic Stress
Average/Derive
Derive/Average
Node 11
28.59
28.59
Invariant Stresses.
1st, 2nd, and 3rd invariant stresses are calculated from the following equations:
σ
1st
=
( σ
x
+
σ
y
+
σ
z
)
σ
2nd
=
σ
x
σ
y
+
σ
y
σ
z
+
σ
z
σ
x
–
( τ
2
x y
+
τ
2
yz
+
τ
2
zx
)
σ
3rd
=
σ
x
( σ
y
σ
z
–
τ
2
yz
)
+
τ
x y
( τ
x y
σ
z
–
τ
yz
τ
z x
)
+
τ
zx
( τ
xy
τ
y z
–
σ
x
τ
z x
)
From the von Mises example above the invariant stresses are:
Invariant Stresses (Node 11)
Average/Derive
Derive/Average
1st Invariant
85.78
85.78
2nd Invariant
374.44
373.38
3rd Invariant
0.00
0.00
13
290
PART 6
Results Postprocessing
13
Principal Stresses.
Principal stresses are calculated from either a Mohr’s circle method for 2D tensors
( σ
z
=
τ
y z
=
τ
z x
=
0
)
or from a 3x3 Jacobian Rotation Eigenvector extraction method for a 3D tensors. The User Interface allows for either a tensor-dependent derivation, or a 2D calculation. The tensor-dependent calculation will choose either a 2D or 3D calculation depending on values of each tensor encountered. A 2D calculation will be used when the ZZ, YZ and ZX are exactly zero (which is the case when the analysis code does not calculate these values), otherwise the full 3D tensor will be considered. Both the magnitudes of the principals and their direction cosines are calculated from these routines.
The magnitudes of the two principal stresses from the 2D Mohr’s circle method are calculated according the following equations:
σ
ma jo r
=
σ
av e
+
( σ
x
–
σ
a v e
)
2
+
τ
2
xy
σ
mi n or
=
σ
a v e
–
( σ
x
–
σ
av e
)
2
+
τ
2
xy
where:
σ
a v e
=
( σ
+
σ
-------------------------
2
)
The direction cosines for the 2D Mohr’s circle method are calculated by assembling the following
3x3 transformation matrix:
– cos
θ sin
θ
0 sin
θ
0 cos
θ
0
0 1
where
θ
= atan
σ
x
τ
–
x y
σ
a v e
--------------------------------------------
2
From the von Mises example above the principal stresses are:
Principal Stresses (Node 11)
Average/Derive
Derive/Average
Maximum
81.17
81.20
4.61
4.58
Minimum
Also the principal stress determinant is the product of the three principals and the major, minor, and intermediate principal deviatoric stresses are calculated from:
σ
( )
=
σ
m a jo r
–
( σ
+
σ
+
σ
-----------------------------------------------------------------------
3
)
σ
( )
=
σ
m i no r
–
( σ
+
σ
+
σ
-----------------------------------------------------------------------
3
)
σ
( )
=
σ
in t er
–
( σ
+
σ
3
+
σ )
-----------------------------------------------------------------------
CHAPTER 14
Numerical Methods
291
Tresca Shear Stress.
Tresca shear stress is calculated from the following equation:
τ
=
( σ
ma j or
–
σ
m i no r
) where
σ
m a jo r
and
σ
m i no r
are calculated as mentioned under Principal stress derivations above.
From the von Mises example above the Tresca shear stress is:
Tresca Shear Stress
Average/Derive
Derive/Average
Node 11
76.55
76.61
Maximum Shear Stress.
Maximum shear stress is calculated from the following equation
τ
=
( σ
–
2
σ ) where
σ
m a jo r
and
σ
m i no r
are calculated as mentioned under Principal stress derivations above.
From the von Mises example above the Tresca shear stress is:
Tresca Shear Stress
Average/Derive
Derive/Average
Node 11
76.55
76.61
Magnitude.
Magnitude (vector length) is calculated from the components with the standard formula:
magn itu de
=
x
2
+
y
2
+
z
2
13
292
PART 6
Results Postprocessing
13
14.4
Averaging
For Fringe and other plots and reports that must display or report values at nodes from elemental data regardless of where the element results are computed, must be converted to results at element nodes. The interpolation functions are then used (e.g., by the graphics module for fringe plot and other operations) to compute the results at any point within the element. The interpolation functions may or may not be the shape functions that were used by the analysis program to compute the element results.
As a rule, each element sharing a common node has its own result values. To compute results for continuous fringe plots, these values need to be averaged and distributed to the sharing elements. The options for the averaging process are described below:
No Averaging
Averaging Based on
All Entities
Averaging Based on
Target Entities
Averaging Based on
Materials
Averaging Based on
Properties
Averaging Based on
Element Types
Difference
Sum
Each element retains its value at the element nodes. Or in other words, each element is its own averaging domain. This selection from the Averaging Domain pull down is called None. The fringe plot will have jumps (not continuous regions) at element boundaries.
All elements will contribute to the sum and will receive the averaged result regardless of whether only certain entities have been selected for the display of the fringe plot. All surrounding elements will contribute to the averaging process.
Only the elements defined as the target entities will contribute to the sum and will receive the averaged result. Surrounding elements that are not part of the target entities will not contribute to the averaging process.
Elements with the same material IDs will contribute to the sum and will receive the averaged result. The fringe plot will have jumps at material boundaries.
Elements with the same property IDs will contribute to the sum and will receive the averaged result. The fringe plot will have jumps at property boundaries.
Elements of the same type will contribute to the sum and will receive the averaged result. The fringe plot will have jumps at element type boundaries.
The minimum and maximum results from the elements sharing a common node are computed. The difference is determined as the delta between the maximum and minimum contributor to each node. The fringe plot of this max difference indicates the quality of the mesh and the location where this mesh needs to be refined by comparing its values with the actual values of the results. Nodal results will have zero max-difference.
The sum of all contributing nodes will be displayed. This step skips the averaging.
CHAPTER 14
Numerical Methods
293
Below are some examples of the averaging techniques. The model in
illustration purposes. It consists of 8 QUAD4 elements and 4 TRI3 elements with a total of 17 nodes.
13
Figure 14-1 Square Plate Model to Illustrate Averaging Techniques.
The above model is also broken up into various material and property sets as such:
Prop1
Prop2
Prop3
Prop4
Target1
Target2
Mat1
Mat2
Mat3
Mat1
Elem 1:3
Elem 6 8:9
Elem 4 7
Elem 10:13
Elem 1:3 6 10:11
Elem 4 7:9 12:13
294
PART 6
Results Postprocessing
13
1
2
3
4
5
6
7
8
9
Node
Element Centroidal Results.
The first illustration is the simple case of results at element
below lists some scalar values of strain energy at each element centroid.
The table is listed by node number with each element and corresponding strain energy value for all contributing elements associated with the particular nodes. The averaging domain columns on the right then list the averaged values for each node based on the averaging domain. Columns with more than one value per node indicate a boundary of the averaging domain and will
therefore cause a plot discontinuity across boundaries. See
averaging domains.
Element
Strain
Energy
3.01
13.06
3.01
4.78
13.06
0.10
0.27
3.01
3.01
4.78
4.78
3.16
3.16
4.78
3.16
2.31
0.10
0.11
3.16
2.31
13.06
11.13
1
2
1
4
4
10
13
2
2
3
3
1
1
4
7
11
3
6
2
3
6
10
Table 14-1 Averaging at Nodes from Element Centroidal Results
Averaging Domain
All
3.01
3.89
3.97
3.16
8.04
4.24
2.09
2.74
12.10
Property Material None
3.01
3.89
3.01
3.89
3.97
3.16
3.01
13.06
3.89
13.06
0.19
3.97
2.31
0.11
3.16
2.31
12.10
3.97
3.16
2.04
13.06
2.04
2.04
2.04
2.04
3.16
2.31
12.10
4.78
3.16
2.31
0.10
0.11
3.16
2.31
13.06
11.13
3.01
13.06
3.01
4.78
13.06
0.10
0.27
3.01
3.01
4.78
4.78
3.16
3.16
Type
3.01
3.89
3.97
3.16
8.04
6.95
0.19
3.42
0.11
2.74
12.10
Target
3.01
3.89
3.97
3.16
3.01
13.06
2.63
6.67
2.63
6.67
2.09
2.74
12.10
CHAPTER 14
Numerical Methods
295
10
11
12
13
14
15
16
17
Node Element
Strain
Energy
0.10
0.11
0.27
0.27
11.13
5.02
5.02
2.82
2.82
2.82
0.11
0.27
2.31
2.82
11.13
13.06
11.13
5.02
0.27
0.27
2.31
5.02
8
9
9
7
8
9
7
9
11
12
6
10
11
12
13
4
7
8
12
13
6
8
Table 14-1 Averaging at Nodes from Element Centroidal Results (continued)
All
5.95
2.11
2.57
11.13
11.13
8.08
3.92
2.82
0.19
Averaging Domain
Property Material None
12.01
5.02
0.27
3.38
0.19
2.57
11.13
5.02
3.92
2.82
0.19
12.01
5.02
0.27
3.38
0.19
2.57
11.13
11.13
5.02
3.92
2.82
0.19
0.10
0.11
0.27
0.27
11.13
5.02
5.02
2.82
2.82
2.82
0.11
0.27
2.31
2.82
11.13
13.06
11.13
5.02
0.27
0.27
2.31
5.02
Type
9.74
0.27
3.38
0.19
2.57
11.13
8.08
3.92
2.82
0.19
Target
5.95
1.21
2.70
1.21
2.31
2.82
11.13
8.08
3.92
2.82
0.10
0.27
13
296
PART 6
Results Postprocessing
13
Element Nodal Results.
The second illustration is the more complex case of results at element nodes.
below is listed by element number with each node and corresponding von
Mises stress for all nodes associated with the particular element. This case is identical to the element centroid case with the exception that each node can have a different value for each contributing element. In this example von Mises stress is derived first and then averaged. See
for visual effects of averaging domains.
1
2
3
4
6
7
Element Node von Mises
Stress
266353
205495
194627
251128
267747
269673
288631
287859
226076
223550
216967
219806
410849
314864
316307
409360
270577
231683
231124
269415
353127
336749
331970
351258
7
6
2
3
3
4
1
2
6
5
8
7
5
6
10
12
11
9
10
14
13
9
7
8
Table 14-2 Averaging at Nodes from Element Nodal Results
All
266353 266353
236621 236621
238950 263404
330989 251128
236621 236621
247874 247874
213334 254218
238950 263404
247874 247874
223550 223550
224325 216967
213334 254218
330989 410849
238950 314864
310705 326528
381243 381243
213334 270577
224325 231683
264210 264210
265760 311763
381243 381243
310705 326528
361658 331970
351258 351258
Averaging Domain
Property Material None
266353
236621
240096
251128
236621
247874
199024
240096
247874
223550
216967
199024
410849
314864
326528
381243
270577
231683
264210
311763
381243
326528
331970
351258
Type
266353 266353
205495 236621
194627 265783
251128 330989
267747 236621
269673 247874
288631 259671
287859 265783
226076 247874
223550 223550
216967 224325
219806 259671
410849 330989
314864 265783
316307 350090
409360 381243
270577 259671
231683 224325
231124 264210
269415 311763
353127 381243
336749 350090
331970 361658
351258 351258
Target
266353
236621
209085
251128
236621
247874
213334
209085
247874
223550
224325
213334
410849
283747
310705
381243
213334
224325
231124
206152
381243
310705
361658
351258
CHAPTER 14
Numerical Methods
297
8
9
Element Node
10
11
12
13
von Mises
Stress
142890
250623
250623
250623
252631
252631
252631
307878
144769
144769
144769
142890
142890
397215
389998
384259
391346
275878
297297
331799
17
11
10
17
10
6
17
15
6
7
17
7
11
10
11
15
14
11
12
16
Table 14-2 Averaging at Nodes from Element Nodal Results (continued)
All
310705 397215
265760 311763
346068 346068
361658 391346
265760 311763
264210 264210
331799 331799
346068 346068
238950 198700
213334 143829
197728 197728
213334 143829
265760 196756
197728 197728
265760 196756
310705 251626
197728 197728
310705 251626
238950 198700
197728 197728
Averaging Domain
Property Material None
197728
196756
251626
197728
251626
240096
197728
346068
240096
199024
197728
199024
196756
397215
311763
346068
391346
311763
264210
331799
Type
397215 350090
389998 311763
384259 346068
391346 361658
275878 311763
297297 264210
331799 331799
307878 307878
144769 198700
144769 143829
144769 197728
142890 143829
142890 196756
142890 197728
250623 196756
250623 251626
250623 197728
252631 251626
252631 198700
252631 197728
Target
143829
305499
310705
251627
310705
283747
251627
346068
209085
213334
143829
213334
206152
310705
305499
346068
361658
305499
297297
331799
13
298
PART 6
Results Postprocessing
13
All Entities By Property By Material
By Element Type None By Target Entity
Figure 14-2 Differences in Plots Due to Averaging Domains - Note Discontinuities.
CHAPTER 14
Numerical Methods
299
14.5
Extrapolation
When element results are provided to MSC.Patran at quadrature points, it is necessary to extrapolate the results from the quadrature points to the nodes of the element and to the element centroid. Similarly, when results are provided at the element nodes or the centroid, it is necessary to interpolate/extrapolate the results to the centroid or nodes respectively.
MSC.Patran has three basic methods to perform this interpolation/extrapolation:
•
By parametric mapping method.
•
By solving a set of equations.
•
By averaging.
The User Interface allows for four basic methods in which the user can control extrapolation methods. These are explained below and examples given.
Shape Function.
If the arrangement of node/quadrature points corresponds to an element type in MSC.Patran, the shape functions are known, and a parametric mapping is used. This is the preferred method, and is the most accurate representation. The parametric mapping method involves mapping the output positions to an element topology that interpolation functions of that topology can be used to compute results at the nodes. As an example, if there are 27 results output at 27 quadrature points inside a hex/20, then these 27 quadrature points can be considered as 27 vertices of a hex/27 element. Results at hex/20 nodes are then computed by the interpolation function of the hex/27, even though these nodes are located outside the element formed by the 27 quadrature points. Once the nodal results of the hex/27 are available, results at the nodes of the hex/20 can be computed by interpolation. These results will be stored in a
20x27 matrix of coefficients. This method only works if there exists an element topology in the library that coincides with the output pattern after being parametrically mapped.
If the arrangement does not correspond to a MSC.Patran element type, a system of equations is constructed and solved for the unknown nodal and centroidal values. The equations are set up such that if the interpolation functions of the element topology are used with the unknown nodal values, they will generate a unit value at each quadrature point. This method only works if there exists an element topology in the library that has the same number of nodes as the number of quadrature points. If Shape Function is set in the User Interface ,the shape functions or a set of equations will be used to extrapolate results as explained above. Only if these two methods fail will averaging take place.
13
300
PART 6
Results Postprocessing
13
Average.
If both previous methods fail, results in the element are averaged and each node of the element will assume this averaged value. Or, alternatively, if the results are provided at nodes, the nodal values would be averaged and assigned to the centroid.
Averaging is also used at element boundaries. In these cases, when extrapolation from different elements yields different result values at the same node, the different results are averaged and assigned to the node.
For degenerate elements, the extrapolation is performed on the parent element topology, and the results at the duplicated nodes in the degenerate element are then averaged.
The User Interface allows for a forced average extrapolation method to be used. The following scenarios can exist.
•
Nodal values to centroid
•
Gauss values to nodes
•
Centroidal values to nodes
Centroid.
A forced extrapolation of the analysis results to the element's centroid can also be set in the User Interface which will be performed relative to where the results are initially located.
Shown below are several different cases that can occur. Once each centroid value is established it is then used to render the results plot.
•
Centroid values to element centroid
•
Nodal values to element centroid
•
Gauss values to element centroid
Min/Max.
The Min/Max method searches each element's results and finds the minimum/maximum value contained within the element. The element then assumes a constant value (including its nodes). For example if the analysis result values are know at the elements
Gauss points the minimum/maximum value is used as a constant value across the element. This method has no effect for results that already exist at the element centroid or the nodes.
CHAPTER 14
Numerical Methods
301
Examples.
Examples are given below for each extrapolation technique using a simple 4 node
QUAD element with four interior Gauss points. The Gauss points are located in parametric space at +/- 0.5773502692 (as per theory). In p/q parametric space, where the extrapolation occurs, would look something like
q axis
1.0
0.5774
Grid 11 Grid 14
13
Grid 12
Gauss Point 1 Gauss Point 4
Centroid
0.5774
1.0
p axis
Gauss Point 2 Gauss Point 3
Grid 13
Figure 14-3 Example 4 Noded QUAD with Gauss Points.
The element will have a simple set of linear shape functions described by
N
1
= –
(
p
– 1
) (
q
+ 1
)
N
2
=
(
p
–
1
) (
q
–
1
)
N
3
= –
(
p
+
1
) (
q
–
1
)
N
4
=
(
p
+
1
) (
q
+
1
)
Using these shape functions, the results at any point in the element would be found as
Result p q
)
=
∑
N i
(
p q
) ×
Resu lt i
where i runs from 1 to 4 for the four Gauss or grid points.
Note that the shape functions vary by element type and element order. The function shown in these examples are not necessarily the functions used in any particular element formulation; they are to illustrate the extrapolation methods only.
302
PART 6
Results Postprocessing
13
Example 1 - Parametric Mapping (Gauss points to element nodes)
Gauss point results are as follows:
3
4
1
2
Gauss Point
10.
15.
20.
15.
Stress
The stress values at the Gauss points will be extrapolated to the grid locations. To do this, the
Gauss points are assigned parametric locations of 1.0. The location of the grids will be at parametric locations of 1/0.5774 or about +/-1.7319 with respect to the Gauss points.
The stress at grid 14, located in parametric space at x/y coordinates of (1.7319, 1.7319) will be calculated as:
–
1
4
(
–
1
+
)
1
4
(
+
1
(
1.7319
+
1
)
) (
1.7319
+
1
×
)
10
×
+
15
1
4
(
–
1
) (
1.7319
–
1
) ×
15
=
15.00
+ –
1
4
(
+
1
) (
1.7319
–
1
) ×
20
The stresses at the rest of the grids would be as follows:
11
12
13
14
Grid X Location
-1.7319
-1.7319
1.7319
1.7319
Y Location
1.7319
-1.7319
-1.7319
1.7319
Stress
6.340499
15.00
23.65950
15.00
Example 2 - Parametric Mapping (Gauss points to element centroid)
The stress at the Gauss points are the same as Example 1. The element centroid would be located in parametric space at (0,0), so interpolation to that point can be accomplished directly:
–
1
4
(
– 1
) (
0 + 1
) ×
10 +
1
4
(
– 1
) (
0 – 1
) ×
15 + –
1
4
(
+ 1
) (
0 – 1
) ×
20 +
1
4
(
+ 1
) (
0 + 1
) ×
15 = 15.00
CHAPTER 14
Numerical Methods
303
Example 3 - Parametric Mapping (Nodal results to element centroid)
In this example the results at the grid points are provided to MSC.Patran. To make an element fill plot, the element centroidal value must be known. The stress values at the element grid points are:
1
2
3
4
Gauss Point Stress
6.340499
15.00
23.65950
15.00
The value at the centroid is then calculated using the shape functions, just as in Example 2 above:
–
1
4
(
–
1
) (
0
+
1
) ×
10
+
1
4
(
–
1
) (
0
–
1
) ×
15
+ –
1
4
(
+
1
) (
0
–
1
) ×
20
+
1
4
(
+
1
) (
0
+
1
) ×
15
=
15.00
Note that this gives the same results as in the previous example.
Example 4 - Averaging (Nodal results to element centroid)
The averaging technique simply computes the mathematical average of the nodal stresses and reports this as the centroidal value. So, the centroidal stress would be reported as:
(
6.340499
+ 15 + 23.65950
+ 15
) ⁄
4 = 15.00
Example 5 - Averaging (Gauss points to element nodes)
In this case no suitable set of shape functions exists to carry out a proper interpolation. Therefore, the Gauss point stresses are averaged, and the average result distributed to all the grid points:
(
10 + 15 + 20 + 15
) ⁄
4 = 15.00
The grid point stresses would be reported as:
11
12
13
14
Grid Point
15.00
15.00
15.00
15.00
Stress
13
304
PART 6
Results Postprocessing
13
Example 6 - Averaging (Centroidal values to element nodes)
In this case there is only one piece of stress data available, so no assumptions about the stress distribution can be made. Therefore, if the element centroid stress is reported as 15.00, the grid point stress will be reported as:
11
12
13
14
Grid Point
15.00
15.00
15.00
15.00
Stress
Example 7 - Averaging (Adjacent element contributions)
In this case the stresses in an adjacent element are included in the reporting of the grid point stress. If two elements have nodal stresses calculated from Gauss points by internal extrapolation as follows:
11
12
13
14
Grid Point
Element 1
Stress
6.340499
15.00
23.65950
15.00
13
14
15
16
Grid Point
Element 2
The nodal stresses calculated by MSC.Patran would be:
27.50
17.50
10.00
9.50
Stress
11
12
13
14
15
16
Grid Point Stress
6.340499
15.00
25.5798 = [ ( 23.65650 + 27.50 ) / 2 ]
16.25 = [ ( 15.00 + 17.50 ) / 2 ]
10.00
9.50
CHAPTER 14
Numerical Methods
305
14.6
Coordinate Systems
Results are stored in the MSC.Patran database in a variety of ways. They are also transformed, either automatically or by the user when necessary, to create meaningful plots. It is important to understand each of these coordinate systems and know in what coordinate system results are stored and whether any transformations are being performed prior to graphical display.
Vectors are transformed as:
v
=
R U
where v is a vector referenced in the local coordinate system defined by the rotation matrix [R], each row of which defines a unit vector in the global system. U is a vector referenced in the global system. For example, if the global system is rotated
θ°
about the z axis, the rotation matrix of the new system is:
= cos
– sin
0 sin cos
0 1
0
0
The inverse vector transformation is:
U
=
T v
which transforms a vector result defined in the [R] system to the global system, since [R] is an orthonormal matrix by definition.
Similarly, the tensors are transformed as:
σ
=
R
[ ]
T
13
The inverse tensor transformation is:
S
=
T
σ
R
For nodal results, the coordinate system types are:
Global system
Nodal system
User system
Type=0
=1
=3
ID=0
=0
=Assigned
306
PART 6
Results Postprocessing
13
For element results, the coordinate system types are:
Global system
Element system
User system
Material system
Ply system
Type=0
=2
=3
=4
=5
ID=0
=0
=Assigned
=0
=0
Global System.
This is the MSC.Patran global or default rectangular coordinate system. For
MSC.Nastran users, this is the same as the MSC.Nastran basic coordinate system. Most alternate coordinate systems use the global system as a basis.
Local Systems.
These are MSC.Patran local coordinate systems specifically created by the user within MSC.Patran. They can be either rectangular, cylindrical, or spherical. These are the same as MSC.Nastran global coordinate systems in MSC.Nastran terminology. Do not be confused by this terminology. Just remember that user defined systems in MSC.Patran are called local systems and user defined systems in MSC.Nastran are called global systems. The default coordinate system in MSC.Patran is called the global system and the default system in
MSC.Nastran is called the basic system.
Reference Systems.
These are local systems or the global system by which geometric definitions are defined. For instance the coordinates locations of a finite element node is defined by referring to a reference system, either local or global.
Analysis Systems.
These are the local systems in which results at finite element nodes will be calculated by the analysis solver. Nodes can be defined in one system (the reference system) but results calculated in another (the analysis system). In general, when nodal results are imported into the MSC.Patran database, they will be stored in the analysis systems.
Unknown Systems.
These are systems which are unknown to MSC.Patran and therefore must remain in these systems when postprocessing. No transformation are allowed.
Element Systems.
These are coordinate systems local to each specific element. There are many types of element coordinate systems. Suffice it to say here, that when elemental based results calculated in an elemental system are imported into the MSC.Patran database, the coordinate systems in which they are stored vary from element to element. This makes meaningful graphical visualization of these results quite difficult. Many times a coordinate transformation is required to convert all results into a consistent coordinate system. Once this is done then operations such as nodal averaging and scalar results derivations (von Mises) can be performed correctly and meaningfully.
CHAPTER 14
Numerical Methods
307
Projected Global System.
This is one system used to convert and display element based shell and plate data stored in an element systems into a consistent, meaningful plot.
The projected global system is defined as follows: First, the normal to the shell surface is calculated. This varies for curved elements and is constant for flat elements. If the angle between the normal and the global x-axis is greater than 0.01 radians, the global x-axis is projected onto the shell surface as the local x-axis. If the angle is less than 0.01 radians, either the global y-axis or the z-axis (whichever makes the largest angle with the normal) is defined to be the local x-axis.
The local y-axis is perpendicular to the plane defined by the normal and the local x-axis. The projected z-axis will align with the element normal.
For one dimensional (1D) and three dimensional (3D) elements, the projected global system is the global system and therefore no projection is performed.
This system has been set as the default for viewing fringe and other plots of element based vector and tensor components on two dimensional (2D) elements. It provides a system with real-world significance which is consistent from element to element.
Projected Systems.
These are systems like the projected global system but instead project other coordinate systems other than the global onto the elements. An example is the shell pelements of MSC.Nastran which use a convective system which is a project of a coordinate system onto the element (plus an optional flip and rotation):
k
= element normal at poing of projection
j
=
k
×
P ax i s
i
=
j
×
k
If projected axis is parallel to element normal, the axis of greatest projection is used.
13
P k
P axis j i
Figure 14-4 Projected Coordinate System Definition.
308
PART 6
Results Postprocessing
13
MSC.Patran Element IJK.
These are MSC.Patran defined element coordinate systems. Many analysis translators will convert results from code specific element coordinate systems to a consistent MSC.Patran element IJK coordinate system. These systems differ from element topology to element topology.The IJK system is defined as follows:
i
=
V
1
k =
V
1
×
V
2
j
=
k
×
i
V
1
=
V
1
–
2
V
2
=
V
1
–
3
v - determined by property for beam or V
1
x {Global y | Global x | Global z},based on least difference V
1 v
Hex
1
8
Bar
V
1
2
7
1
4
Quad
V
V
1
2
4
3
2
V
2
3
1
Tri
4
V
1
Wedge
6
2
5
5
4
6
Tet
V
2
3
V
2
3
V
2
3
1
2
1
V
1
2
V
1
1
V
1
2
Figure 14-5 MSC.Patran Element IJK Coordinate System Definitions.
Element Bisector (CQUAD4).
This element coordinate systems, supported by MSC.Patran, is specific to the MSC.Nastran CQUAD4 element. Other element types default to the IJK system.
The definition of the bisector system is as follows:
i =
V
1
+
V
2
j
=
V
1
–
V
2
CHAPTER 14
Numerical Methods
309
k = i
×
j
j
4
3
V
1
CQUAD4 k out of plane i
V
2
1
2
Figure 14-6 CQUAD4 Bisector Coordinate System Definition.
Material Systems.
These are element coordinate systems based on a material definition and angle. These exist for QUAD and TRI elements only. Material coordinate systems are defined as follows:
i
=
V
1
rotated
α
about k which is rotated around a degrees about k. a is from the material property record.
j
=
k
×
i
The k vector is the same as that for bisector (QUAD element) or IJK (TRI element).
3
V
2 j
Tri
4
Quad j i
1
α
α
k
- out of plane
2
1 k
- out of plane
V
1
V
1 i
Figure 14-7 MSC.Patran Element IJK Coordinate System Definitions.
3
2
13
310
PART 6
Results Postprocessing
MSC.Nastran CQUAD8 System.
This element coordinate systems, supported by MSC.Patran, is specific to the MSC.Nastran CQUAD8 element. Other element types default to the IJK system.
This coordinate system is position dependent. The definition of this system is as follows:
n
= element normal at a position
13
t
1
=
2
= tangent 2
Use bisections:
b
1
=
t
1
+
t
2
b
2
=
n
+
b
1
So the element system is:
i
=
j
×
k
j
=
b
1
+
b
2
k
=
n
CQUAD8
8
4 n
7 t
2 t
1
6
3
1
5
2
Figure 14-8 MSC.Nastran CQUAD8 Coordinate System Definition.
CHAPTER 14
Numerical Methods
311
MSC.Nastran CTRIA6 System.
This element coordinate systems, supported by MSC.Patran, is specific to the MSC.Nastran CTRIA6 element. Other element types default to the IJK system.
This coordinate system is position dependent. The definition of this system is as follows:
n
= element normal at a position
t
1
= tangent 1
So the element system is:
i =
t
1
j
=
n
×
i
k
=
n
13
3
6
CTRIA6 n
5 t
1
4
1
2
Figure 14-9 MSC.Nastran CTRIA6 Coordinate System Definition.
312
PART 6
Results Postprocessing
13
MSC.Patran Reference Manual, Part 6: Results Postprocessing
CHAPTER
15
Verification and Validation
■
■
314
PART 6
Results Postprocessing
14
15.1
Overview
The purpose of this chapter is to demonstrate the correctness of result postprocessing plots, graphs, reports, and result combinations and derivations in MSC.Patran. A number of representative models are used to illustrate this validation and verification. In most cases very simple models are used for simplicity and clarity. Many of these models have closed form solution which are compared to the finite element solutions as displayed in MSC.Patran. The main purpose of this chapter, however, is to show that MSC.Patran correctly displays results as reported and calculated by the finite element solver. It is not to prove that any particular finite element solver calculates the correct answers.
Care has been taken to ensure that as much functionality as possible is covered by these examples. As new postprocessing capabilities are added to MSC.Patran from release to release, this chapter will increase its scope. Each problem gives a description of pertinent information that any engineer should be aware of when postprocessing results. These include:
❏
Solver and solution type
❏
Element type
❏
Model and result descriptions
❏
Postprocessing features covered
All problem files have been provided with the MSC.Patran delivery and are indicated with each
problem if the user wishes to investigate them personally. below gives a brief description of each
problem. These files are located in a directory in the main MSC.Patran installation directory called:
<install_dir>/results_vv_files
Problem
Table 15-1. V&V Problems
Description
MSC.Nastran, Solution 101, Linear
Statics, Deformation and Fringe
Plots of Displacement Results.
MSC.Nastran, Solution 101, Linear
Statics, Fringe Plots of Cross-Ply
Stress Results with Coordinate
Transformation to Global System.
MSC.Nastran, Solution 101, Linear
Statics, Fringe and Tensor Plots of
Stress Tensor and Principal
Stresses in Beam.
MSC.Nastran, Solution 101, Linear
Statics, Displacement Plots and
Fringe Plots of Stress and
Displacement with Local
Coordinate Transformations.
Features Validated
prob001.bdf
prob001.op2
prob002.bdf
prob002.op2
prob003.bdf
prob003.op2
prob004.bdf
prob004.op2
CHAPTER 15
Verification and Validation
315
Table 15-1. V&V Problems
Problem
Problem 12: Nonlinear Statics,
Problem 13: Nonlinear Statics,
Description
MSC.Nastran, Solution 101, Linear
Statics, Deformation and Fringe
Plots of Stress with Spherical
Coordinate Transformations.
MSC.Nastran, Solution 101, Linear
Statics, Deformation and Fringe
Plots of Stress Using Axisymmetric
Elements.
MSC.Nastran, Solution 101, Linear
Statics, Repeat of Problem 6 Using
Solid Elements and Cylindrical
Frame.
MSC.Nastran, Solution 101, Linear
Statics, Displacement Plots and
Fringe Plots of Deflection, Stress and Rod Forces.
MSC.Nastran, Solution 106, Non-
Linear Statics, Large
Displacements, Displacement
Fringe Plots of Deflection of a Plate
Modeled with CQUAD4 and
CQUAD8, CTRIA3 and CTRIA6
Element Types.
Features Validated
prob005.bdf
prob005.op2
prob006.bdf
prob006.op2
prob007.bdf
prob007.op
prob008.bdf
prob008.op2
prob009_Q4.bdf
prob009_Q4.op2
prob009_Q8.bdf
prob009_Q8.op2
prob009_T3.bdf
prob009_T3.op2
prob009_T6.bdf
prob009_T6.op2
prob010.bdf
prob010.op2
MSC.Nastran, Solution 101, Linear
Statics, Fringe Plots Stress due to
Thermal Gradient.
MSC.Nastran, Solution 101, Linear
Statics, Fringe Plots of Deflection and Linear Superposition.
prob011_A.bdf
prob011_A.op2
prob011_B.bdf
prob011_B.op2
prob011_C.bdf
prob011_C.op2
MSC.Nastran, Solution 106, Non-
Linear Statics, Displacement,
Fringe and Vector Plots of
Deflection.
MSC.Nastran, Solution 106, Non-
Linear Statics, Displacement and
Fringe Plots of Deflection.
MSC.Nastran, Solution 103,
Normal Modes, Vector Plots of
Mode Shapes.
prob012.bdf
prob012.op2
prob013.bdf
prob013.op2
prob014.bdf
prob014.op2
14
316
PART 6
Results Postprocessing
14
Table 15-1. V&V Problems
Problem
Problem 17: Buckling, shells and Cylindrical Coordinates
Motion with Modal Damping and Rigid Body Elements
Motion with Modal Damping and Shell P-Elements
Description
MSC.Nastran, Solution 103,
Normal Modes, Deformation and
Fringe Plots of Mode Shapes using h-Element Formulation.
MSC.Nastran, Solution 103,
Normal Modes, Deformation and
Fringe Plots of Mode Shapes using p-Element Formulation.
MSC.Nastran, Solution 105,
Buckling, Deformation and Fringe
Plot of Buckled Cylinder.
MSC.Nastran, Solution 105,
Buckling, Deformation and Fringe
Plot of Buckled Plate.
MSC.Nastran, Solution 109, Direct
Transient Response, Graph and
Fringe Plots of Responses.
Features Validated
prob015.bdf
prob015.op2
prob016.bdf
prob016.op2
prob017.bdf
prob017.op2
prob018.bdf
prob018.op2
prob019_T.bdf
prob019_T.op2
prob019_S.bdf
prob019_S.op2
MSC.Nastran, Solution 112, Modal
Transient Response, Graph and
Plots of Responses.
prob020.bdf
prob020.op2
MSC.Nastran, Solution 129,
Nonlinear Transient Response,
Graph Plots of Responses.
MSC.Nastran, Solution 129,
Nonlinear Transient Response,
Graph Plots of Responses.
prob021.bdf
prob021.op2
prob022.bdf
prob022.op2
MSC.Nastran, Solution 108 Direct
Frequency Response, Graph Plots of Responses.
MSC.Nastran, Solution 103 & 111,
Modal Frequency Response,
Fringe Plots of Mode Shapes,
Graph Plots of Responses.
MSC.Nastran, Solution 111, Modal
Frequency Response, Graph Plots of Responses.
prob023_1.bdf
prob023_1.op2
prob023_2.bdf
prob023_2.op2
prob023_3.bdf
prob023_3.op2
prob024_1.bdf
prob024_1.op2
prob024_2.bdf
prob024_2.op2
prob025.bdf
prob025.op2
CHAPTER 15
Verification and Validation
317
Table 15-1. V&V Problems
Problem
Description
MSC.Nastran, Solution 107,
Complex Modes, Direct Method,
Fringe and Deformation Plots of
Modes.
MSC.Nastran, Solution 153, Steady
State Heat Transfer, Fringe Plots of
Temperature and Radiation Heat
Flux.
MSC.Nastran, Solution 159,
Transient Thermal Analysis, Graph
Plots of Temperature Responses.
MSC.Nastran, Solution 153, Steady
State Heat Transfer, Fringe Plots of
Temperatures.
MSC.Nastran, Solution 101, Linear
Statics, Freebody Plots.
Features Validated
prob026.bdf
prob026.op2
prob027.bdf
prob027.op2
prob028.bdf
prob028.op2
prob029.bdf
prob029.op2
prob030.bdf
prob030.op2
14
318
PART 6
Results Postprocessing
14
15.2
Validation Problems
Problem 1: Linear Statics, Rigid Frame Analysis
Solution/Element Type:
MSC.Nastran, Solution 101, Linear Statics, CBAR Bar Elements with Standard Formulation
Reference:
Roark, R.J., and Young, W.C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, pp. 122-126.
Problem Description:
A rigid frame with uniform properties is subjected to a concentrated force midspan of the top horizontal member. One end of the frame is fixed while the other is free. Find the horizontal and vertical displacements as well as the rotation at the free end of the frame.
Engineering Data:
l
1
= 7.0in
l
2
=
10.0in
l
3
=
4.0in
a
=
2.0in
E
=
E
1
=
E
2
=
E
3
=
10
7
psi v
=
0.3
I
=
I
1
=
I
2
=
I
3
= 0.0052083in
4
W
=
100.0lbf
CHAPTER 15
Verification and Validation
319
Theoretical Solution:
Upon substitution of the engineering data into the equations below, the following results are obtained:
δ
HA
= –
W l
2
(
1
–
l
2
) (
l
3
–
a
)
+
l
1
3
–
a
)
2
= – 0.10368in
Source
MSC.Nastran
*
Theory
%, Difference
δ
V A
= –
W
l l
---------
EI
3
2
+
3
l
--------- a
3EI
–
l
2
l
---------
EI
3
–
l
---------
2EI
2
+
3
---------
= –
0.16640in
Ψ
A
= –
W l
------ l
EI
(
33
–
a
)
+
2EI
33
–
a
)
2
= – 0.0422403radians
MSC.Nastran Results:
To determine the deflections at the free end of the frame, the model shown in
was created. This model consisted of 14 MSC.Nastran CBAR elements. Each bar was assumed to have a square cross-section of 0.5 x 0.5 inches. This gives a cross-sectional moment of inertia of
0.0052083 in4 that is identical to what was assumed in the preceding calculations. Using this model, the following results were obtained.
Table 15-2 Rigid Frame Analysis Results
δ
HA
0.10368
-0.10368
0.0%
δ
V A
-0.16706
-0.16664
0.252%
Ψ
A
0.042243
-0.042240
0.007%
*MSC.Nastran results have opposite sign due to the reversal of the direction of x and z axes of the global coordinate frame relative to the theoretical results coordinates.
The corresponding deformed shape plot that was made for the rigid frame is shown in
where the deformed shape has been superimposed upon the undeformed mesh.
Fringe plots for the x, y, and z components of the translational displacements that were generated with MSC.Patran are shown in
,
respectively. The fringe plot for the rotation about the z axis is shown plotted in
fringe plots are displayed on the fully deformed structure. Examination of these fringe plots near the free end of the frame clearly shows that the MSC.Patran results are identical to the preceding
MSC.Nastran results.
File(s):
<install_dir>/results_vv_files/prob001.bdf, prob001.op2
14
320
PART 6
Results Postprocessing
14
Basic Model
Load and BCs
Figure 15-1 Basic FE Model of Rigid Frame with Load and BCs.
Deformed and Undeformed Shape
Figure 15-2 Deformed and Undeformed Shape of Rigid Frame.
X-Translation
Figure 15-3 X-Translational Deformation of Rigid Frame.
CHAPTER 15
Verification and Validation
321
14
Y-Translation
Figure 15-4 Y-Translational Deformation of Rigid Frame.
322
PART 6
Results Postprocessing
14
Z-Translation
Figure 15-5 Z-Translational Deformation of Rigid Frame.
Rotation About Z-Axis
Figure 15-6 Rotational Displacement about Z-axis of Rigid Frame.
CHAPTER 15
Verification and Validation
323
Problem 2: Linear Statics, Cross-Ply Composite Plate Analysis
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CQUAD4 Elements with Standard Formulation and
Laminated Material Properties.
Reference:
Jones, R. M., Mechanics of Composite Materials, Hemisphere Pub. Corp., 1975, pp. 198-201.
Problem Description:
A flat rectangular plate is made from a cross-ply 0/90/0 degree ply stacking. Assuming that the plate is cured at 270 o
F, find the stress in each of the plies once the plate is cooled down to 70 o
F.
14
Engineering Data:
length
=
l
= 3.0in
width
=
w
=
2.0in
laminate thickness
=
t
= 0.55in
outer ply thickness
=
t o
=
0.0458in
inner ply thickness
=
t i
= 0.4583in
N x
=
200lb
f
⁄ in
E
1
=
7.8
×
10
6
psi
E
2
= 2.6
×
10
6
psi
G
12
=
1.25
×
10
6
psi v
12
=
0.25
α
1
=
3.5
×
10
– 6
⁄ °
F
α
2
= 11.4
×
10
–
6
⁄ °
F
Theoretical Solution:
Only the stresses in plies 1 and 2 are shown since the laminate is symmetric about its midplane.
Hence, ply 1 is identical to ply 3. In the expressions below,
∆
T
refers to the temperature difference between the curing temperature for the laminate and its final operational temperature. In this particular example,
∆
T
would equal -200 o
F. Because of the absence of any localized restraint to thermal shrinkage coupled with isotropic thermal expansions, the stresses in each ply are uniform. The predicted stresses are as follows for
N x
=
,
∆
T
= –
200
°
F
324
PART 6
Results Postprocessing
14
σ
1
x
( )
=
2.27
N
------
t x
+
35.5
∆
T
-------
F
= –
6274.55psi
σ
1
y
( )
=
0.12
N
------
t x
–
16.0
∆
T
-------
F
=
3243.64psi
σ
2
x
( )
= 0.75
N
------
t x
– 7.1
∆
T
-------
F
= 1692.73psi
σ
2
y
( )
= – 0.024
N x
------
t
+ 3.2
∆
T
-------
F
= – 648.73psi
τ
1
x y
( )
=
τ
2
x y
( )
=
0
MSC.Nastran Results:
To predict the stresses in the cross-ply laminate for this problem, a model was created that consisted of CQUAD4 elements with laminate properties specified by a MSC.Nastran PCOMP data entry. This permitted stress recovery to be performed on a ply by ply basis. Due to symmetry, any motion along the vertical and horizontal planes of symmetry was restrained out.
In addition, all out of plane deformations were restrained since a balanced cross-ply laminate should remain flat during cool down. Application of these boundary conditions avoided any potential problems with unrestrained rigid body motion. The applied loads and boundary conditions are also shown superimposed upon the finite element mesh in
.
Using this model, the following results were obtained with MSC.Nastran.
Source
MSC.Nastran
Theory
%, Difference
Table 15-3 Ply Stress,
σ
x
σ
x
-6280.51
-6274.55
0.095%
σ
x
1691.68
1692.73
-0.062%
σ
x
-6280.51
6274.55
0.095%
Source
MSC.Nastran
Theory
%, Difference
Source
MSC.Nastran
Theory
%, Difference
Table 15-4 Ply Stress,
σ
y
σ
y
3228.55
3243.64
-0.465%
σ
y
-645.29
-648.73
-0.530%
Table 15-5 Shear Stresses,
τ
τ
x y
-0.002043
0.0
-
τ
x y
0.000551
0.0
-
σ
y
3228.55
3243.64
-0.465%
τ
x y
-0.002043
0.0
-
CHAPTER 15
Verification and Validation
325
The corresponding fringe plots that were generated with MSC.Patran for the x-, y- and xy shear
stress components in each of the plies are shown in
through
. A comparison of these plots with the preceding MSC.Nastran results clearly shows that the two are identical. Layer 1 and 3 were plotted in the element coordinate system; layer 2 was plotted in the
Global coordinate system. You must read in the .bdf file below to be able to perform the correct coordinate transformation to reproduce the layer 2 plots.
Files:
<install_dir>/results_vv_files/prob002.bdf, prob002.op2
14
Basic Model
Figure 15-7 Basic Cross-Ply FE Composite Plate Model.
326
PART 6
Results Postprocessing
XX Stress - Layer 1
14
Figure 15-8 Cross-Ply Composite Plate,
σ
x
Stress, Layer 1.
YY Stress - Layer 1
Figure 15-9 Cross-Ply Composite Plate,
σ
y
Stress, Layer 1.
XY Stress - Layer 1
Figure 15-10 Cross-Ply Composite Plate,
τ
x y
Stress, Layer 1.
XX Stress - Layer 2
CHAPTER 15
Verification and Validation
327
14
Figure 15-11 Cross-Ply Composite Plate,
σ
x
Stress, Layer 2.
328
PART 6
Results Postprocessing
YY Stress - Layer 2
14
Figure 15-12 Cross-Ply Composite Plate,
σ
y
Stress, Layer 2.
XY Stress - Layer 2
Figure 15-13 Cross-Ply Composite Plate,
τ
x y
Stress, Layer 2.
XX Stress - Layer 3
Figure 15-14 Cross-Ply Composite Plate,
σ
x
Stress, Layer 3.
YY Stress - Layer 3
CHAPTER 15
Verification and Validation
329
14
Figure 15-15 Cross-Ply Composite Plate,
σ
y
Stress, Layer 3.
330
PART 6
Results Postprocessing
XY Stress - Layer 3
14
Figure 15-16 Cross-Ply Composite Plate,
τ
x y
Stress, Layer3.
CHAPTER 15
Verification and Validation
331
Problem 3: Linear Statics, Principal Stress and Stress
Transformation
Solution/Element Type:
MSC.Nastran, Solution 101, Linear Statics, CQUAD4 Elements with Standard Formulation.
Reference:
Popov, E.P., Introduction to Mechanics of Solids, Prentice-Hall, Inc., 1968, pp. 337-340.
Roark, R.J., and Young, W.C. , Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, pp.
62, 93 - 96, 101.
Problem Description:
A weightless rectangular beam spans 40 inches and is loaded with a vertical downward force W
= 18.44 kips at midspan. Find the principal stresses at points a, b, c, b
’
and a
’
.
y
10”
W=18.44 kips
20”
1.535” a b c x
6”
5.75”
12” b’
A
B a’
14
Engineering Data:
Length
=
l
= 40in
Height
=
h
=
12in
Depth
=
d
=
1.535in
v
= 0.318
Theoretical Solution:
Reaction Loads:
R
A
=
W l
(
–
a
)
=
18.44
40
(
–
20
)
=
9.22kips
R
B
=
l
=
40
=
9.22kips
I
1
=
dh
3
⁄
12
=
221.04in
4
I
2
=
hd
3
⁄
12 = 3.617in
4
E
= 3
×
10
7
psi
332
PART 6
Results Postprocessing
14
Transverse Shear Force:
V
=
R
A
–
⟨
–
a
⟩
0
=
R
A
=
9.22kips where
⟨
x
–
a
⟩
0
=
0
1
x
<
a x
>
a undefined
x=a
Moments:
M
A
=
M
B
=
0
=
R
A x
–
(
–
a
) ⟨
x
–
a
⟩
0
M
10
=
R
A
=
92.2Kips
–
in
⟨
–
a
⟩
0
=
(
= 10
) < (
a
= 20
)
Fiber and Shear Stresses:
σ (
x y
)
=
I
=
[
R
–
(
–
I a
) ⟨
x
–
a
⟩
0
]
y
--------------------------------------------------------------------
τ
x y
=
VA
′
y
′
Id
Here A’ is the area of that part of the section above (or below if the point of interest is located below the beam’s neutral axis) the point of interest and y’ is the distance from the neutral axis to the centroid of A’ as shown below.
Stress at a:
σ (
10 6
)
=
–
R xy
----------------
I
=
–
( )
10
( )
221.04
= –
2.50ksi
τ
x y
( )
=
0.0
CHAPTER 15
Verification and Validation
333
Stress at b:
σ (
10 5.5
)
τ
x y
(
=
–
R
A xy
----------------
I
=
–
( )
10
(
5.5
)
221.04
= –
2.29
ksi
)
= –
VA
′
y
′
Id
= –
(
9.22
(
)
10
(
0.5
) (
5.75
221.04
) (
1.535
)
)
= –
0.12ksi
Stress at c:
σ (
10 0
)
=
0.0
τ
x y
= –
VA
′
y
′
Id
=
(
9.22
(
) (
1.535
221.04
)
6 3
) (
1.535
)
( )
= – 0.75ksi
Stress at b’:
σ (
10
,
– 5.5
)
=
–
R xy
----------------
I
=
–
( )
10
(
– 5.5
)
221.04
= 2.29ksi
τ
x y
(
10
,
–
5.5
)
=
VA
′
y
′
Id
=
(
9.22
(
) (
1.535
221.04
)
)
(
(
0.5
) (
1.535
–
)
5.75
)
= –
0.12ksi
Stress at a’:
σ (
10
,
–
6
)
=
–
R xy
----------------
I
=
–
(
τ
x y
=
0.0
)
10 6
221.04
=
2.50ksi
Based upon these fiber and shear stresses, the following principal stresses are calculated:
14
a b b c c b’ b’ a’
334
PART 6
Results Postprocessing
14
MSC.Nastran Results:
To determine the stress state in the beam, a MSC.Nastran model was generated using
MSC.Patran. To maximize accuracy, a mesh density was chosen so that nodes would be precisely situated at every designated stress recovery point. In addition, to prevent any out of plane deformation, all displacements normal to the plane of the model were fully restrained, thereby imposing a plane strain condition. Furthermore, to prevent any longitudinal rigid body translation, a symmetry boundary condition was imposed at midspan the entire height of the
beam. The imposed boundary conditions and applied loads are shown in
superimposed upon the mesh, which consisted solely of CQUAD4 elements using a standard formulation. Using this model, the following stresses were predicted at points a, b, c, b’ and a’.
Source
MSC.Nastran
Theory
%, Difference
Table 15-6 Stresses* at Position a
σ
x
-2354.
-2500.
-5.85%
τ
x y
-64.04
0.0
-
Max Principal
-29. 75
0.0
-
Min Principal
-2356.
-2500.
-5.76%
Source
MSC.Nastran
Theory
%, Difference
Table 15-7 Stresses* at Position b
σ
x
-2151.
-2290.
-6.07%
τ
x y
-124.4
-120.0
3.67%
Max Principal
12.65
6.00
110.8%
Min Principal
-2158.
-2298.
-6.09%
Source
MSC.Nastran
Theory
%, Difference
Source
MSC.Nastran
Theory
%, Difference
Table 15-8 Stresses* at Position c
σ
x
-122.9
0.0
-
τ
x y
-760.1
-750.0
1.35%
Max Principal
756.5
750.0
0.867%
Table 15-9 Stresses* at Position b’
σ
x
2437.
2290.
6.42%
τ
x y
-106.5
-120.0
-11.3%
Max Principal
2442.
2298.
6.27%
Min Principal
-779.9
-750.0
3.99%
Min Principal
1.557
6.00
-74. 05%
CHAPTER 15
Verification and Validation
335
Table 15-10 Stresses* at Position a’
Source
MSC.Nastran
Theory
%, Difference
σ
x
2671.
2500.
6.64%
τ
x y
-54.92
0.0
-
* Based upon nodal average of adjacent elements.
Max Principal
2672.
2500.
6.88%
Min Principal
40.86
0.0
-
The MSC.Patran fringe plots that were made of the x-, y- and xy- stress components are shown
show the stress state at each of the designated stress recovery points, tensor plots were made of the fiber stress as well as the principal stress at each position, starting with a and proceeding onto
a’
. Examination of the MSC.Patran
tensor and fringe plots reveals that they are identical to the preceding MSC.Nastran results.
File(s):
<install_dir>/results_vv_files/prob003.bdf, prob003.op2
14
Basic Model
Figure 15-17 Basic Beam Model with Loads and Boundary Conditions.
336
PART 6
Results Postprocessing
14
XX Stress
Figure 15-18
σ
x
Stress of Beam Model.
YY Stress
Figure 15-19
σ
y
Stress of Beam Model.
XY Stress
Figure 15-20
τ
x y
Stress of Beam Model.
CHAPTER 15
Verification and Validation
337
14
Zero Shear Angle
Figure 15-21 Orientation Angle of Maximum Principal Stress.
338
PART 6
Results Postprocessing
Point a Stress Tensor
14
Point b Stress Tensor
Figure 15-22 Stress Tensor at Points a and b.
Point a Principal Stresses Point b Principal Stresses
Figure 15-23 Principal Stresses at Points a and b.
Point a’ Stress Tensor Point b’ Stress Tensor
CHAPTER 15
Verification and Validation
339
14
Figure 15-24 Stress Tensor at Points a’ and b’.
Point a’ Principal Stresses Point b’ Principal Stresses
Figure 15-25 Principal Stresses at Points a’ and b’.
340
PART 6
Results Postprocessing
Point c Stress Tensor
14
Point c Principal Stresses
Figure 15-26 Stress Tensor and Principal Stresses at Point c.
Problem 4: Linear Statics, Plane Strain with 2D Solids
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CQUAD4, CQUAD8, CTRIA3, CTRIA6, CQUADR and CTRIAR Elements with Standard and Revised Formulations
Reference:
Roark, R. J., and Young, W. C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, p.
504.
Problem Description:
An infinitely long, thick walled, cylinder is subjected to a uniform internal pressure. Assuming near incompressible material behavior, find the radial displacement as well the radial and hoop stress at the inner diameter (ID) and outer diameter (OD) of the cylinder.
CHAPTER 15
Verification and Validation
341
Engineering Data:
E=1000. psi
v
=
0.4999
a = 9.0 inches b = 3.0 inches q = 100. psi
Theoretical Solution:
For the case of an internally pressurized thick walled cylinder, the displacement and stresses at the inner and outer radius are given by the equations below. Upon substituting the assumed values for
E
, , , , and q , the following displacements and stresses are calculated:
σ
1
= 0
σ
2
=
r
2
(
a
2
(
2
+
r
–
b
2
)
2
)
=
25.00psi , r=a
125.00psi , r=b
max
σ
2
=
2
q a
2
+
–
b
2
b
2
σ
3
=
–
2
(
a
2
r
2
(
a
2
–
–
r
2
)
b
2
)
=
–
0 , r=a
100.0p
si
, r=b
max
σ
3
= –
q
at r=b
∆
a
=
E
2ab
2
------------------
a
2
–
b
2
=
0.2250inches
∆
b
=
E a
2
2
+
b
2
v a
–
b
2
+ =
0.5250inches
MSC.Nastran Results:
For the purposes of this problem, a 15 degree segment was modeled of the cross-section of the pipe with the appropriate axisymmetric boundary conditions being applied to the lateral edges of the model. In addition, five individual segments were modeled that were meshed with either
CQUAD4, CQUAD8, CTRIA3 or CTRIA6 elements using a standard formulation or CQUADR and CTRIAR elements with a revised formulation. This was done to assess how variations in element topology and formulation affect overall accuracy of the results when performing a plane strain analysis with a high Poisson’s ratio. The actual model that was generated with
MSC.Patran is shown in
where the individual element types associated with each segment have been identified. The loading and boundary conditions that were applied to the
14
342
PART 6
Results Postprocessing
14
Using the aforementioned model, the following results were obtained for each of the various element types.
MSC.Nastran*
Theory
%, Difference
Table 15-11 Displacement,
∆
a
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
.1370
.2250
-39.11%
.1690
.2250
.1680
.2250
.1689
.2250
-24.89% -25.33% -24.93%
.1755
.2250
-22.00%
.1726
.2250
-23.29%
MSC.Nastran*
Theory
%, Difference
Table 15-12 Displacement,
∆
b
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
.4102
.5250
-21.87%
.5060
.5250
-3.62%
.5031
.5250
-4.17%
.5058
.5250
-3.66%
.5357
.5250
2.04%
.5256
.5250
0.11%
MSC.Nastran*
Theory
%, Difference
MSC.Nastran*
Theory
%, Difference
MSC.Nastran*
Theory
%, Difference
Table 15-13 Stresses,
σ
=
a
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
-165.1
25.00
-760.40%
25.32
25.00
1.28%
25.00
25.00
0.0%
25.01
25.00
0.04%
25.30
25.00
1.20%
26.44
25.00
5.76%
Table 15-14 Stresses,
σ
=
b
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
1766.
125.00
1312.8%
129.4
125.00
3.52%
124.0
125.00
-0.80%
124.3
125.00
-0.56%
131.7
125.00
5.36%
129.3
125.00
3.44%
Table 15-15 Stresses,
σ
=
a
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
-186.0
0.0
-
.3775
0.0
-
.7289
0.0
-
.0476
0.0
-
3.809
0.0
-
-3.039
0.0
-
CHAPTER 15
Verification and Validation
343
MSC.Nastran*
Theory
%, Difference
Table 15-16 Stresses,
σ
=
b
CQUAD4 CQUAD8 CTRIA3 CTRIA6 CQUADR CTRIAR
1591.0
-100.0
1691%
-94.52
-100.0
- 6.48%
-91.00
-100.0
-9.00%
-99.47
-100.0
-.53%
-52.96
-100.0
-47.04%
-119.6
-100.0
19.60%
* Represents average of all edge nodal values with nodal values averaged across adjacent elements.
The fringe plot that was generated for the radial displacement is shown in
plots for the radial and hoop stress are shown in
stresses have been plotted with an adjusted scale that better shows the stress gradient present in each of the segments. All plots have been transformed into the cylindrical coordinate system defined in the problem. A comparison with the preceding tabular results clearly shows that
MSC.Patran is accurately reproducing the MSC.Nastran results.
The preceding results clearly demonstrate the wide degree of variability in the result attributable to element topology as well as formulation. Consistently, the higher order CQUAD8 and
CTRIA6 elements gave superior performance compared to their linear counterparts. Similarly, in this application where cylindrical geometry was involved, a triangular element gave far more accurate results then compared to a quadrilateral element. Only by adopting the revised formulation of a CQUADR could acceptable results be obtained with a quadrilateral element.
This would not be unexpected since the removal of any membrane-bending coupling produces far less sensitivity to extreme values in Poisson’s ratio as in this example.
File(s):
<install_dir>/results_vv_files/prob004.bdf, prob004.op2
14
CTRIA6 CTRIA3
CQUADR
CQUAD8
CTRIAR
CQUAD4
Figure 15-27 Basic Models Using 2D Solid Elements.
344
PART 6
Results Postprocessing
14
Figure 15-28 Loads and Boundary Conditions of 2D Solid Models.
Radial Displacments
Figure 15-29 Fringe Plot of Radial Displacement on 2D Solids.
CHAPTER 15
Verification and Validation
345
14
Radial Stresses
Figure 15-30 Fringe Plot of Radial Stress,
σ
3
, on 2D Solid Elements.
Hoop Stresses
Figure 15-31 Fringe Plot of Hoop Stress,
σ
2
, on 2D Solid Elements.
346
PART 6
Results Postprocessing
14
Problem 5: Linear Statics, 2D Shells in Spherical Coordinates
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CQUAD4 and CTRIA3 with Standard Formulation
Reference:
Roark, R. J., and Young, W.C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, p.
451.
Problem Description:
A section of a thin, spherical shell is internally pressurized. The free edge of the shell is restrained in the meridional direction. Find the stresses and displacements of the shell.
Engineering Data:
t = 0.05 in
R
2
= 10.0 in
q = 200.0 psi
θ
=
45.0 degrees
E = 1.0 x 10
7
psi
υ
= 0.333
Theoretical Solution:
For the case of an internally pressurized spherical shell tangentially supported, the predicted stresses and displacements are, after substituting the assumed values for
E
, , , and R
2
:
σ
1
=
σ
2
=
qR
2t
=
∆
R
2
=
qR
2
(
1
---------------------------
2Et
–
v
)
= 0.013340in
∆
y
=
qR
2
(
1
–
v
) (
2Et
1
– cos
θ )
= 0.003907in
∆
R
=
qR
2
(
1 –
2Et
v
) sin
θ
=
0.009433in
MSC.Nastran Results:
A model of the spherical shell was created using MSC.Patran. Due to symmetry, only one fourth of the shell was modeled with the appropriate axisymmetric boundary conditions applied to the
free edges. The model that was created is shown in
. The majority of the model was
CHAPTER 15
Verification and Validation
347
meshed with CQUAD4 elements, with the mesh becoming increasingly refined near the center of the shell. Only at the very apex of the shell are CTRIA3 elements used. However, every attempt was made to minimize having high aspect ratio triangular elements that would otherwise cause a loss of accuracy. Using this model, the following results were obtained.
Source
Theory
MSC.Nastran
%, Difference
Table 15-17 2D Shell Displacements
∆
R
2
∆
R
max
.01334
.01462
9.60%
min
.01334
.01383
3.67%
.009433
.010330
9.51%
∆
y
.003907
.003890
0.435%
Table 15-18 2D Shell Stresses*
Source
Theory
MSC.Nastran
%, Difference max
20,000.
20,034.
0.170%
σ
1
min
20,000.
19,881.
0.595%
max
20,000.
20,563.
2.82%
* Based upon nodal averaging of results between adjacent elements.
σ
2
min
20,000.
19,877.
0.615%
The corresponding fringe plots for the radial displacement and the x-displacement in global coordinates are shown in
and
. The radial displacement plot gives
∆
R
2
whereas the max value shown on the x-displacement plot corresponds to
∆
R
, the y-displacement in global coordinates is plotted. The difference between the maximum
and minimum y-displacements corresponds to
∆
y
above, or the change in vertical height for the shell. Fringe plots for the radial, meridional and circumferential stresses are shown in
. A comparison of the MSC.Patran fringe plots with the MSC.Nastran
results shows an exact correlation between the two.
14
348
PART 6
Results Postprocessing
File(s):
<install_dir>/results_vv_files/prob005.bdf, prob005.op2
14
Basic Model
Figure 15-32 Basic Model of 2D Shell in Spherical Coordinates.
Radial Displacements
Figure 15-33 Radial Displacement of Spherical Membrane.
Global X Displacements
Figure 15-34 Global Translational X Displacement of Membrane.
Global Y Displacements
CHAPTER 15
Verification and Validation
349
14
Figure 15-35 Global Translational Y Displacement of Membrane.
350
PART 6
Results Postprocessing
14
Radial Stresses
Figure 15-36 Radial Stresses of Spherical Membrane.
Meridional Stresses
Figure 15-37 Meridional Stresses of Spherical Membrane.
CHAPTER 15
Verification and Validation
351
14
Circumerential Stresses
Figure 15-38 Circumferential Stresses of Spherical Membrane.
Problem 6: Linear Statics, 2D Axisymmetric Solids
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CTRIAX6 Elements, 2D Axisymmetric Solids
Reference:
Roark, R. J., and Young, W. C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, pp. 504-505.
Problem Description:
A thick walled cylinder with thick end caps is subjected to a uniform external pressure.
Determine both the radial and hoop displacement and stress state at the mid plane of the cylinder.
352
PART 6
Results Postprocessing
14
Engineering Data:
E = 1.0 x 10
7
psi
υ
= 0.333
a = 6.0 in b = 4.0 in l = 11.0 in t = 0.5 in q = 1000.0 lb/in
2
Theoretical Solution:
For the case of an externally pressurized thick walled cylinder with thick end caps, there is no closed form solution. The nearest solution corresponds to a capped thick walled cylinder where the restraint afforded by the end caps to radial and hoop contraction is ignored. The presence of the thick end caps would necessarily reduce the radial and hoop displacement at the mid plane of the cylinder, resulting in lower axial and hoop stresses. Only the radial stress would be left unaltered at the mid plane. However, a substantial gradient in all of the stress components should be observed near the ends of the cylinder due to bending of the end caps. Nevertheless, the classical closed form solution is useful in bounding the actual displacements and stresses and is as follows. For the assumed values for
E
υ
a b
and q
, the following results are obtained for an externally pressurized thick walled cylinder with negligible end caps:
σ
1
=
–
a
2
–
2
b
2
= –
1800psi
σ
2
=
r
2
2
(
(
a a
2
2
–
+
r
2
b
2
)
)
= –
2600 psi at
r
=
a
=
6.0inches max
σ
2
=
2
q a
2
+
–
b
2
b
2
= – 3600 psi at
r
=
b
= 4.0inches
CHAPTER 15
Verification and Validation
353
σ
3
=
–
qb
2
(
r
2
(
a
2
2
–
–
r
2
)
b
2
)
=
0 psi at r
=
b
=
4.0inches max
σ
3
= –
q
= – 1000 psi at
r
=
a
= 6.0inches
∆
a
=
–
E
2
(
1
–
2v
)
a
2
–
+
b
2
(
1
+
v
)
b
2
= –
0.001006inches
∆
b
=
–
E
2
(
a
2
2
–
v
)
–
b
2
= – 0.001202inches
∆
l
=
–
E
2
(
a
2
–
b
2
)
= – 0.000673
inches
MSC.Nastran Results:
Two models were created with MSC.Patran of the thick walled cylinder. One featured 3 noded and the other 6 noded CTRIAX6 elements. Both models used the same number of elements. The
models with the applied loading are shown in
uniform external ambient pressure of 1000.0 psi. Using these models, results were obtained and the following errors occurred relative to the theoretical values for each of the element topologies that were examined. The results clearly show the expected behavior; namely, the presence of the end caps reduces the inward radial contraction at the center of the cylinder. This necessarily reduces the predicted hoop stress relative to the theoretical value. The only stress components that should correlate with the theoretical values are the radial stress at the ID and OD of the cylinder ad the axial stress at the mean radius of the cylinder.
Theory
MSC.Nastran
% Difference
Table 15-19 Radial Stress,
σ
3
*
3 Noded CTRIAX
r = a r = b
-1000.0
-903.576
-9.64%
0.0
-268.901
-
6 Noded CTRIAX
r = a r = b
-1000.0
-1000.697
0.0697%
0.0
-9.847213
-
Theory
MSC.Nastran
% Difference
Table 15-20 Hoop Stress,
σ
2
*
3 Noded CTRIAX
r = a
-2600.0
-2363.289
-9.104%
r = b
-3600.0
-2967.001
-17.58%
6 Noded CTRIAX
r = a
-2600.0
-2467.246
-5.12%
r = b
-3600.0
-2740.299
-23.88%
14
354
PART 6
Results Postprocessing
Theory
MSC.Nastran
% Difference
Table 15-21 Axial Stress at Mean Diameter,
σ
1
*
3 Noded CTRIAX
-1800.0
-1871.255
3.96%
6 Noded CTRIAX
-1800.0
-1876.067
4.23%
14
Table 15-22 Displacements*
Theory
MSC.Nastran
% Difference
∆
a
3 Noded CTRIAX
∆
b
∆
l
∆
a
6 Noded CTRIAX
∆
b
∆
l
-1.006E-3 -1.202E-3 -6.73E-4 -1.006E-3 -1.202E-3 -6.73E-4
-7.986E-4 -9.586E-4 -6.340E-4 -8.104E-4 -9.814E-4 -6.297E-4
-25.97% -20.247% -6.145% -19.441% -18.354% -6.873%
* Results based upon nodal average of adjacent elements.
The fringe plots created of the radial displacement are shown in
.
The range has been adjusted to better show the displacement at the center of the cylinder.
Similarly, the radial stress distribution is shown in
stress in
; and the axial stress in
and
A comparison of the MSC.Patran fringe plots with the preceding tabular results clearly reveals that the MSC.Nastran results are being accurately displayed.
File(s):
<install_dir>/results_vv_files/prob006.bdf, prob006.op2
CHAPTER 15
Verification and Validation
355
14
Basic Models
One 3 Noded
One 6 Noded
Figure 15-39 Axisymmetric Models of Thick Walled Cylinder.
Radial Displacement
6 Noded CTRIAX Elements
Figure 15-40 Radial Displacement of 6 Noded Axisymmetric Model.
356
PART 6
Results Postprocessing
14
Radial Displacement
3 Noded CTRIAX Elements
Figure 15-41 Radial Displacement of 3 Noded Axisymmetric Model.
Radial Stresses
6 Noded CTRIAX6 Elements
Figure 15-42 Radial Stress in 6 Noded Axisymmetric Model.
CHAPTER 15
Verification and Validation
357
Radial Stresses
3 Noded CTRIAX ELements
Figure 15-43 Radial Stress in 3 Noded Axisymmetric Model.
14
Hoop Stresses
6 Noded CTRIAX Elements
Figure 15-44 Hoop Stress in 6 Noded Axisymmetric Model.
358
PART 6
Results Postprocessing
14
Hoop Stresses
3 Noded CTRIAX Elements
Figure 15-45 Hoop Stress in 3 Noded Axisymmetric Model.
Axial Stresses
6 Noded CTRIAX Elements
Figure 15-46 Axial Stress in 6 Noded Axisymmetric Model.
CHAPTER 15
Verification and Validation
359
Axial Stresses
3 Noded CTRIAX Elements
Figure 15-47 Axial Stress in 3 Noded Axisymmetric Model.
14
360
PART 6
Results Postprocessing
14
Problem 7: Linear Statics, 3D Solids and Cylindrical Coordinate
Frames
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CHEX8 Elements - 3D Solids
Reference:
Roark, R.J., and Young, W. C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, pp.
504-505.
Problem Description:
Problem 6: Linear Statics, 2D Axisymmetric Solids
exception that the cylinder and end caps are entirely modeled with MSC.Nastran 3D solid HEX8 elements. In addition, all analytical results are recovered in a global cylindrical coordinate frame.
This should produce results that are identical to those recovered with CTRIAX6 2D axisymmetric solid elements.
Engineering Data:
E = 1.0 x 10
7
psi
υ
= 0.333
a = 6.0 in
b = 4.0 in
l = 11.0 in
t = 0.5 in
q = 1000.0 psi
Theoretical Solution:
Problem 6: Linear Statics, 2D Axisymmetric Solids
(p. 351) for derivation and theoretical
results.
MSC.Nastran Results:
A model was created of the thick walled cylinder with the end caps using just MSC.Nastran 3D solid CHEX8 elements. Due to symmetry, only one eighth of the cylinder was modeled, with the appropriate axisymmetric and symmetry boundary conditions applied to the free faces of the
model. The model that was created is shown in
. Using this model, the results below were computed at the middle of
the cylinder.
CHAPTER 15
Verification and Validation
361
Once again, the analytical results demonstrate the expected behavior. Namely, the presence of the end caps reduces the inward radial contraction at the center of the cylinder. This reduces the predicted hoop stress relative to the theoretical value. The only stress components that are unaffected are the radial stress at the ID and OD of the cylinder and the axial stress at the mean radius of the cylinder. The percent error that occurred relative to the theoretical values for the radial and axial stress are shown below. For comparative purposes, the results that were obtained for a three noded CTRIAX6 element have been included, illustrating the excellent degree of correlation that exists when using either element type to model axisymmetric structures.
Theory
MSC.Nastran
% Difference
Table 15-23 Radial Stresses,
σ
3
*
r = a
-1000.0
-918.731
-8.13%
CHEX8
r = b
0.0
-184.862
-
CTRIAX6, 3 Noded
r = a r = b
-1000.0
-903.576
-9.64%
0.0
-268.901
-
Theory
MSC.Nastran
% Difference
Theory
MSC.Nastran
% Difference
Table 15-24 Hoop Stresses,
σ
2
*
r = a
-2600.0
-2902.487
11.634%
CHEX8
r = b
-3600.0
-2418.523
-32.819%
CTRIAX6, 3 Noded
r = a
-2600.0
-2467.246
-5.12%
r = b
-3600.0
-2740.299
-23.88%
Table 15-25 Axial Stresses,
σ
1
*
CHEX8
-1800.0
-1760.235
-2.21%
CTRIAX6, 3 Noded
1800.0
1871.255
3.96%
Table 15-26 Displacements*
Theory
MSC.Nastran
% Difference
∆
a
CHEX8
∆
b
∆
l
∆
a
CTRIAX6
∆
b
∆
l
-1.006E-3 -1.202E-3 -6.73E-4 -1.006E-3 -1.202E-3 -6.73E-4
-8.095E-4 -9.980E-4 -6.043E-4 -8.104E-4 -9.814E-4 -6.297E-4
-19.535% -18.346% -10.212% -19.441% -18.354% -6.873%
* Results based upon nodal average of adjacent elements.
14
362
PART 6
Results Postprocessing
14
The corresponding fringe plots that were generated for the radial and axial displacement are shown in
. Similarly, fringe plots for the radial, hoop and axial
stress are shown in
,
, respectively. In each of the fringe plots, the range has been purposely adjusted to better show the gradient in displacement and stress that exists at the middle of the cylinder. In addition, all stresses and displacements have been transformed to a cylindrical coordinate frame. If the boundary conditions were properly applied, then an axisymmetric response should be present, which is evident in each of fringe plots.
File(s):
<install_dir>/results_vv_files/prob007.bdf, prob007.op2
Basic Model
Figure 15-48 Solid Model of Thick Walled Cylinder with End Caps.
Applied Loads and BCs
Figure 15-49 Loads and Boundary Conditions of Cylinder.
CHAPTER 15
Verification and Validation
363
14
Radial Displacement
Figure 15-50 Radial Displacements of Thick Walled Cylinder.
364
PART 6
Results Postprocessing
14
Axial Displacement
Figure 15-51 Axial Displacement of Thick Walled Cylinder.
Radial Stresses
Figure 15-52 Radial,
σ
3
, Stress of Thick Walled Cylinder.
Hoop Stresses
Figure 15-53 Hoop,
σ
2
, Stress of Thick Walled Cylinder.
CHAPTER 15
Verification and Validation
365
14
Axial Stresses
Figure 15-54 Axial,
σ
1
, Stress of Thick Walled Cylinder.
366
PART 6
Results Postprocessing
14
Problem 8: Linear Statics, Pinned Truss Analysis
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CROD 1D Elements.
Reference:
Przemieniecki, J.S., Theory of Matrix Structural Analysis, McGraw-Hill, Inc., 1968, p. 155.
Problem Description:
A pinned joint truss is loaded with a force at one end and one of the components is heated uniformly to an elevated temperature. Considering thermal effects, find the displacements of the truss joints and the forces and stresses in each of the axial elements.
Engineering Data:
E
= 1.0
×
10
7
α
=
1.0
×
10
– 6
/ Deg F
A
1
= 1.0""in
2
(Elements 1,3,5 and 6)
A
2
=
0.7071068""in
2
(
Elements 2 and 4
)
∆
T
=
100.Deg F (Elements 3 only)
F
=
1000.0lb.
6
1
2
4
3 v1 v2 u1
T
l
=
20.in
5 u2
Theoretical Solution:
The theoretical solution was calculated by using the matrix equation on page 159 of the reference using the values listed above for
F
, , and
∆
T
. The results are as follows:
Displacements:
u
1
= –
1.272727
×
10
–
3 in
v
1
=
+6.363636
×
10
– 3 in
u
2
=
+7.272727
×
10
–
4 in
v
2
=
+3.636364
×
10
– 3 in
CHAPTER 15
Verification and Validation
367
Element Forces:
P i
=
EA u l
×
i
P1 = -636.36 lb (compression)
P
2
= +899.95 lb (tension)
P
3
= +363.64 lb (tension)
Element Stresses:
σ
1
=
P
1
/ A
1
= – 636.36 lb/in
2
σ
2
=
P
2
/A
2
= +1272.73 lb/in
2
σ
3
=
P
3
/A
1
=
+363.64 lb/in
2
P
P
P
4
5
6
= -514.25 lb (compression)
= +363.64 lb (tension)
= 0. lb
σ
4
=
P
4
/ A
2
= – 727.27 lb/in
2
σ
5
=
P
5
/A
5
= +363.64 lb/in
2
σ
6
=
P
6
/A
6
=
0. lb/in
2
MSC.Nastran Results:
Due to the pinned construction of the truss, all members are only capable of carrying axial loads.
This necessitated that the truss be modeled using MSC.Nastran 1D CROD elements. The model that was created using MSC.Patran is shown in
. Note that each truss member was
modeled using a single CROD element. The loads and boundary conditions that were applied to the model are also shown in
The following results were obtained with MSC.Nastran.
Theory
MSC.Nastran
% Difference
Table 15-27 Displacements, (inches) u
1
-1.272727x10
-3
-1.272727x10
-3
0.0%
v
1
+6.363636x10
+6.363636x10
0.0%
-3
-3
u
2
+7.272727x10
-4
+7.272727x10
-4
0.0%
v
2
+3.636364x10
-3
+3.636364x10
-3
0.0%
Theory
MSC.Nastran
% Difference
Table 15-28 Rod Forces (lbs)
P
1
P
2
P
3
P
4
P
5
-636.36
+899.95
+363.64
-514.26
+363.64
-636.36
+899.95
+363.64
-514.26
+363.64
0.0% 0.0% 0.0% 0.0% 0.0%
P
6
0.
0.
0.0%
Theory
MSC.Nastran
% Difference
Table 15-29 Rod Stresses (psi)
σ
1
σ
2
σ
3
σ
4
σ
5
-636.36
+1272.73
+363.64
-727.27
+363.64
-636.36
+1272.73
+363.64
-727.27
+363.64
0.0% 0.0% 0.0% 0.0% 0.0%
σ
6
0.
0.
0.0%
14
368
PART 6
Results Postprocessing
14
The corresponding color fringe plots that were made in MSC.Patran of the x- and y-components of displacement are shown in
, respectively. For the purposes of these plots, the target entity was set to nodes and the averaging domain was specified as all entities. The rod forces and stresses that were predicted by MSC.Nastran are shown in
, respectively. Unlike displacements, it was necessary to set the target entity to elements and the averaging domain to individual. This avoided having any averaging across adjacent elements which otherwise would have given an inaccurate representation of the actual results. A closer inspection of these plots reveals that the results that are being shown are in fact identical to those predicted by MSC.Nastran.
File(s):
<install_dir>/results_vv_files/prob008.bdf, prob008.op2
Basic Model with Loads and BCs
Figure 15-55 Basic Pinned Truss Analysis Model.
X Displacements
CHAPTER 15
Verification and Validation
369
14
Figure 15-56 X Translational Displacement of Pinned Truss.
Y Displacements
Figure 15-57 Y Translational Displacement of Pinned Truss.
370
PART 6
Results Postprocessing
14
Rod Forced
Individual
Figure 15-58 Rod Forces from Pinned Truss Analysis.
Rod Stresses
Individual
Figure 15-59 Axial Stresses from Pinned Truss Analysis.
CHAPTER 15
Verification and Validation
371
Problem 9: Nonlinear Statics, Large Deflection Effects
Solution/Element Type:
MSC.Nastran, Nonlinear Statics, Solution 106, Shell Element with Standard Formulation,
CQUAD4 and CQUAD8
Reference:
Timoshenko, S., and Woinowsky-Krieger, S., Theory of Plates and Shells, McGraw-Hill, Inc., 1959, p. 422.
Problem Description:
A square plate with clamped edges is loaded uniformly such that the center deflection exceeds the plate thickness. Considering large deflection effects (small strain theory), find the deflection at the center of the plate.
a
=
b
=
100.0
h
=
1.0
E
= 2.0
×
10
11
v
= 0.3
q
=
2.0
×
10
4
d
=
3
(
–
v
2
)
=
1.83
×
10
10
14
Theoretical Solution:
The following diagram summarizes the theoretical solution for the case when large deflection effects are both considered and ignored.
For
q
⋅
b
4
⁄ (
Dh
)
=
For
q
⋅
b
4
⁄ (
Dh
)
=
m a x
⁄
h
= 1.20
, with nonlinear effects.
m a x
⁄
h
=
2.208
, without nonlinear effects.
372
PART 6
Results Postprocessing
14
MSC.Nastran Results:
Due to symmetry, only one-fourth of the plate was modeled. The outer edges were fully restrained while the appropriate symmetry boundary conditions were imposed along the remaining free edges and at the center of the plate. Two models were created. The first was meshed with MSC.Nastran CQUAD4 elements which have a finite strain formulation needed to incorporate large deflection effects. The second model was meshed with CQUAD8 elements, which do not have a finite strain formulation. Both models along with the applied loading and imposed boundary conditions are shown in
results that were obtained are summarized below and plotted in
Element Type
QUAD4
QUAD8
Table 15-30 Large Deflection Results
w m ax
⁄
h
(Theory)
,
1.20
2.208
w m ax
⁄
h
,
(MSC.Nastran)
1.26
2.21
% Difference
5.0%
.091%
It should be noted that although both analyses were conducted using MSC.Nastran, Solution 106 with large deflection effects included, the analysis performed with CQUAD8 excluded any geometric nonlinearities since this type of element has no finite strain formulation. This illustrates the care that must be exercised when performing a nonlinear statics analysis with mixed element types. The same problem exists for CTRIA3 and CTRIA6 elements.
File(s):
<install_dir>/results_vv_files/prob009_Q4.bdf, prob009_Q4.op2, prob009_Q8.bdf, prob009_Q9.op2, prob009_T3.bdf, prob009_T3.op2, prob009_T6.bdf, prob009_T6.op2
CQUAD4 Model with Loads and BCs
CHAPTER 15
Verification and Validation
373
Figure 15-60 CQUAD4 Model of Plate with Loads and BCs.
14
CQUAD8 Model with Loads and BCs
Figure 15-61 CQUAD4 Model of Plate with Loads and BCs.
Deflection of CQUAD4 Model
Figure 15-62 Large Deflection Displacements of CQUAD4 Model.
374
PART 6
Results Postprocessing
Deflection of CQUAD8 Model
14
Figure 15-63 Large Deflection Displacements of CQUAD8 Model.
CHAPTER 15
Verification and Validation
375
Problem 10: Linear Statics, Thermal Stress with Solids
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, Solid Elements With Standard Formulation, CHEXA
(8 and 20 noded), CPENTA (6 and 15 noded), CTETRA (4 and 10 noded).
Reference:
Timoshenko, S., and Goodier, J. N., Theory of Elasticity, 2nd ed., McGraw-Hill, Inc., 1951, pp. 401-
403.
Problem Description:
Six cubes are subjected to three independent linear temperature gradients in the x-, y- and z- directions. The cubes are meshed with either HEX8, HEX20, WEDGE6, WEDGE15,
TET4 or TET10 elements. Each cube is mounted on a weak elastic foundation so that the resultant thermal expansion is unrestrained. Compute the Von Mises stress in each of the cubes.
Theoretical Solution:
In general, when the applied temperature is a linear function of x, y and z, the strain induced by free thermal expansion is:
ε
x
=
ε
y
=
ε
z
=
α
T
γ
x
=
γ
y
=
γ
z
=
0
(a)
The corresponding stress-strain relationships for three dimensional problems are:
ε
x
–
α
T
=
1
E
[ σ
x
–
v
( σ
y
+
σ
z
) ]
ε
y
–
α
T
=
1
E
[ σ
y
–
v
( σ
x
+
σ
z
) ]
ε
z
–
α
T
=
1
σ
E
[
z
–
v
( σ
x
+
σ
y
) ]
(b)
(c)
γ
x y
=
τ
-------,
G
γ
y z
=
τ
y z
------- ,
G
γ
z x
=
τ
z x
-------,
G
Equations (c) are not affected by temperature since free thermal expansion does not produce angular distortion in an isotropic material. The remaining stress-strain relationships given by equations (b) can only be satisfied after substitution of the strains due to free thermal expansion if
σ
x
=
σ
y
=
σ
z
=
0
Thus, a linear temperature gradient should produce no apparent stress, provided the expansion is completely unrestrained.
14
376
PART 6
Results Postprocessing
14
MSC.Nastran Results:
To demonstrate that thermal stress effects can be properly recovered for all of the various solid element topologies supported by MSC.Nastran, a simple model was created that consisted of 6 cubes. Each cube was subjected to three independent linear temperature gradients of 100, 200 and 300 degrees F per inch along the x, y and z axes, respectively. The cubes were meshed with either HEX8, HEX20, WEDGE6, WEDGE15 TET4 or TET10 elements with a mesh density of one
element per edge. The model that was created is shown in
temperatures are shown in
.
Due to the presence of three simultaneous temperature gradients, the faces of the cubes will not remain planar. This precludes applying uniform constraints along any face of the cubes in order to prevent any rigid body translation from occurring. Instead every vertex of a cube was attached to a triad of three weak grounded springs that were aligned in either the x, y or zdirections. Each spring had a spring rate of 0.1 lbs / inch, which would provide minimal resistance to thermal expansion. This should generate only a minimal amount of residual stress in each of the cubes.
The maximum von Mises stress that was computed by MSC.Nastran for a given element topology are summarized below.
Table 15-31 Maximum von Mises Stress
Element Type
HEX8
HEX20
WEDGE6
WEDGE15
TET4
TET10
Max Von Mises Stress (psi)
.001512
.007403
49811
.007900
7610
.005904
The corresponding deformed shapes and von Mises stress contours that were generated using
MSC.Patran are shown in
and
, clearly showing the high residual
stresses that were generated in both the degenerate WEDGE6 and TET4 elements. The peak
values for the von Mises stress shown are somewhat less than those shown in due to the nodal
averaging of results at adjacent elements.
Ideally, the presence of a weak elastic support should have provided minimal restraint to thermal expansion, resulting in a near zero stress state. This behavior was observed in both the
HEX8 and HEX20 elements as well as the higher order TET10 and WEDGE15 elements. The extremely high stresses observed with TET4 and WEDGE6 elements would not be unexpected since these elements tend to be excessively stiff resulting in a loss of accuracy. Consequently, the results illustrate the care that must be exercised when modeling with the solids and the need to avoid excessive use of degenerate elements, especially in areas where high stress gradients are predicted to occur, such as at the vertices of the cubes in this particular problem.
File(s):
<install_dir>/results_vv_files/prob010.bdf, prob010.op2
CHAPTER 15
Verification and Validation
377
HEX8
HEX20
WEDGE6
WEDGE15
TET4
TET10
14
Figure 15-64 Models of Different Solid Element Types.
Applied Thermal Gradient
Figure 15-65 Thermal Gradient Applied to Solid Elements.
378
PART 6
Results Postprocessing
14
Deformed Shapes
Figure 15-66 Deformed Shape of Elements Due to Thermal Gradient.
von Mises Stress
Figure 15-67 von Mises Stress in Elements due to Thermal Gradient.
CHAPTER 15
Verification and Validation
379
Problem 11: Superposition of Linear Static Results
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, Simple Shell Elements, CQUAD4 and CTRIA3
Reference:
Ugural, A.C., Stresses in Plates and Shells, McGraw-Hill, Inc., 1981, pp. 41-42.
Roark, R.J., and Young, W.C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Inc., 1975, p.
338.
Problem Description:
A flat annular plate is subjected to a uniform pressure. The inner edge is free and the outer edge simply supported. Determine the maximum deflection of the plate.
Theoretical Solution:
The resultant deformation for a simply supported annular plate can be derived by summing the deformations obtained for a flat circular plate subjected to the same pressure load, an annular plate carrying along its inner edge a shear force per unit circumferential length of annular plate with a distributed radial bending moment of p
o
(
3
+
v
) (
a
2
–
b
2
)
/16 p
o
b/2 and an
. All of the plates have the same outer radius and the both annular plates have the same inner radius.
14
Subcase A Subcase B Subcase C
According to reference (2), the maximum deflection occurs at the inner radius and is given by the expression:
w ma x
=
–
4
p a
---------------
D
C L
---------------
–
L
C
7
11
Eq. 15-1 where
C
1
=
1 +
2
v
ln
a
+
1
–
v b
–
---
a
Eq. 15-2
380
PART 6
Results Postprocessing
14
L
17
=
4
–
1 –
4
v
–
a
4
–
a
2
1
+
(
1
+
v
) ln
b
C
7
=
1
2
(
–
v
2
)
b
–
a
Eq. 15-3
Eq. 15-4
L
11
=
1
4
64
+
a
2
–
5
a
4
–
4
a
2
2
+
a
2 ln
b
Eq. 15-5
D
=
--------------------------
(
Et
12 1 –
3
v
2
)
Eq. 15-6
For the purposes of this problem, models of a flat circular and annular plates where created in
MSC.Patran using the following dimensions, applied loading and material properties:
a
=
8.0 in
b
= 4.0 in
t
= 0.25 in
E
= 1.0
×
10
7
psi
v
= 0.33
p o
= 50.0 psi
MSC.Nastran Results:
The model that was generated for a uniformly pressurized circular plate is shown in
. Due to symmetry, only a 90 degree sector of the plate was modeled with axisymmetric
boundary conditions being applied along the lateral edges of the sector. The center of the plate was constrained to move only in the vertical direction. Between the inner and outer radius of the annular plate, a mesh consisting of CQUAD4 elements was used to maximize accuracy.
Conversely, inboard of the inner radius, a CTRIA3 mesh was used to avoid having badly distorted CQUAD4 elements that might otherwise result in a loss of accuracy. By having the mesh transition coincide exactly with the edges of the annular plate, this permitted using a single model to investigate the behavior of a complete circular plate as well as an annular plate, with the elements corresponding to just the annular and the complete plate being assigned to a different groups within MSC.Patran. The corresponding models that were used to investigate the case of an annular plate subjected to either a distributed edge shear or moment are shown in
.
Due to axisymmetric response of the plate, all deformations are principally confined to the vertical, or z-direction. The resultant vertical displacements as well as the hoop and radial stresses that were computed for each of the three different subcases are shown in
. The displacement and stress contours have been superimposed upon an
exaggerated deformed shape. The resultant displacements and stresses that were derived by
combining the results from each of the separate subcases are shown in
indicates that a maximum deformation of -
0.8799 inches occurs at the inner radius of a flat annular plate subjected to a uniform pressure of
50 psi. Note that for the combined stress plots, the averaging was set to Target Entities to remove the influence of the stresses from the CTRIA3 elements.
CHAPTER 15
Verification and Validation
381
Substitution of the model parameters into equations
maximum deflection at the inner radius of
w m a x
= -0.8839 in
The value derived within MSC.Patran was -.8799 in, or a deviation of approximately 0.69% from the theoretical value
File(s):
<install_dir>/results_vv_files/prob011_A.bdf, prob011_A.op2, prob011_B.bdf, prob011_B.op2, prob011_C.bdf, prob011_C.op2
14
Circular Plate Model with Pressure Loading
Figure 15-68 Model of Pressurized Circular Plate (Subcase A).
382
PART 6
Results Postprocessing
14
Annular Plate with Edge Shear
Figure 15-69 Annular Plate with Edge Shear (Subcase B).
Annular Plate with Edge Moment
Figure 15-70 Annular Plate with Edge Moment (Subcase C).
CHAPTER 15
Verification and Validation
383
14
Subcase A Vertical Displacement
Figure 15-71 Vertical Displacement of Circular Plate (Subcase A).
Radial Stress Subcase A
Figure 15-72 Radial Stress of Circular Plate (Subcase A).
384
PART 6
Results Postprocessing
14
Hoop Stress Subcase A
Figure 15-73 Hoop Stress of Circular Plate (Subcase A).
Vertical Displacement Subcase B
Figure 15-74 Vertical Displacement of Annular Plate (Subcase B).
Radial Stress Subcase B
Figure 15-75 Radial Stress of Annular Plate (Subcase B).
CHAPTER 15
Verification and Validation
385
14
Hoop Stress Subcase B
Figure 15-76 Hoop Stress of Annular Plate (Subcase B).
386
PART 6
Results Postprocessing
14
Vertical Displacements Subcase C
Figure 15-77 Vertical Displacement of Annular Plate (Subcase C).
Radial Stresses Subcase C
Figure 15-78 Radial Stress of Annular Plate (Subcase C).
Hoop Stresses Subcase C
Figure 15-79 Hoop Stress of Annular Plate (Subcase C).
CHAPTER 15
Verification and Validation
387
14
Combined Vertical Displacements
Figure 15-80 Combined Vertical Displacements of Annular Plate.
388
PART 6
Results Postprocessing
14
Combined Radial Stresses
Figure 15-81 Combined Radial Stress of Annular Plate.
Combinded Hoop Stresses
Figure 15-82 Combined Hoop Stress of Annular Plate.
CHAPTER 15
Verification and Validation
389
Problem 12: Nonlinear Statics, Post-Buckled Column
Solution/Element Type:
MSC.Nastran, Nonlinear Statics, Solution 106, CBEAM, 1D Beams with Standard Formulation.
Reference:
Timoshenko, S. P., and Gere, J. M., Theory of Elastic Stability, McGraw-Hill, Inc., 1961, p. 48.
Problem Description:
Find the displaced position of a post-buckled column, fixed at one end with an applied axial load at the other end.
Engineering Data:
l
= 20.0 inches
h
= 1.0 inch
d
=
0.05 inch
E
=
1
×
10
8
psi
v
=
.333
α
=
60
°
I
1
=
(
1/12
)
dh
3
=
4.20
×
10
–
3
in
4
I
2
=
(
1/12
)
hd
3
= 1.04
×
10
– 5
in
4
y l o p x2
A ya x
Theoretical Solution:
The post-buckled beam end coordinates and critical buckling load are given by the equations below. The integrals and are known as the complex elliptical integral of the first and second kind, respectively. Their values are typically listed as a function of sin
-1
(p). For a known deflection angle of
α
=60
0
, the required the load and tip deflection can be derived as shown here
:
P
=
k
2
EI
=
(
0.0843
)
2
(
1
×
10
8
) (
4.2
×
10
–
3
)
= 2984.73 lb
x a
= --- E p
l k
– =
0.0843
)
–
20
=
y a
=
k
=
2 0.5
)
0.0843
=
11.8624 in
14.8161 in
P c r
=
2
EI
4l
2
=
2
(
1
×
10
8
) (
4.2
×
10
– 3
)
4 20
2
)
=
2590.77 lb
14
390
PART 6
Results Postprocessing
14
where:
=
∫
2
0
1
–
p
2
( sin
φ )
2
d
φ
=
E
( sin
–
1
)
=
E
(
30
°
)
=
1.4675
k
=
l
=
20
)
=
0.0843 in
– 1
=
∫
0
2
1 –
p
2
1
( sin
φ )
2
d
φ
=
K
( sin
– 1
)
=
K
(
30
°
)
= 1.6858
p
= sin
2
{ sin
–
1
=
α
/2=30
°
}
= sin
(
30
°
)
=
1/2
MSC.Nastran Results:
To determine the post-buckled shape for the beam, the model shown in
was generated using MSC.Patran. The model consisted of 20 1D CBEAM elements that used a standard generalized formulation. To ensure that the beam will deflect laterally, a slight horizontal load was applied to the beam in addition to an axial load of 2984.73 lbs. In this case a lateral load of 10 lbs was used. In addition, since the structure is post-buckled, it is inherently unstable. This requires that the user set the MSC.Nastran parameter TESTNEG to -2 in the input file.
The following results were obtained with MSC.Nastran.
Source
MSC.Nastran
Theory
%, Difference
Table 15-32 Results of Post-Buckled Beam Deflections
x a
14.4076
14.8161
-2.7571%
y a
12.2275
11.8624
3.0778%
α
62.3583
o
60.0 o
3.9305%
The corresponding MSC.Patran fringe plots that were made of the horizontal and vertical
. Deflection plots were set to
True Scale as opposed to a percentage of the model. The rotation about the global z-axis given in radians is shown in
. For the purposes of evaluating the accuracy of these plots,
it is necessary to use the following conversions:
∆
x
=
y a
∆
y
=
x a
–
20.
CHAPTER 15
Verification and Validation
391
where
∆
x
and
∆
y
are the MSC.Nastran horizontal and vertical nodal displacements, respectively. Vector plots of the translational and rotational displacements are shown in
. After making the appropriate conversions, it is apparent that the MSC.Patran results are identical to those obtained with MSC.Nastran.
File(s):
<install_dir>/results_vv_files/prob012.bdf, prob012.op2
14
Basic Model with Load and BC
Figure 15-83 Nonlinear Beam Post-Buckling Model.
392
PART 6
Results Postprocessing
14
Horizontal Deflection
Figure 15-84 Post-Buckled Horizontal Deformation of Beam.
Vertical Deflection
Figure 15-85 Post-Buckled Vertical Deformation of Beam.
Rotational Displacement
Figure 15-86 Post-Buckled Rotational Deformation about Z of Beam.
Tip Translations
CHAPTER 15
Verification and Validation
393
14
Figure 15-87 Vector Plot of Tip Deflections of Beam.
394
PART 6
Results Postprocessing
14
Tip Rotations
Figure 15-88 Vector Plot of Rotational Deformation of Beam.
CHAPTER 15
395
14
396
PART 6
Results Postprocessing
14
Verification and Validation 15 MSC/PATRAN User’s Guide, Part 6: Results Postprocessing
Problem 13: Nonlinear Statics, Beams with Gap Elements
Solution Type:
MSC.Nastran, Nonlinear Statics, Solution 106. Normal Modes, CBEAM and CGAP
Reference:
McCormac, J.C., Structural Analysis, 3rd ed., New York: Intext Educational Publishers, 1975, p.
323, ex. 17.12.
Problem Description:
A simply supported beam is hinged at one end and supported by lifting rollers at two other locations. Allowing for lift-off to occur, determine the vertical deflections under the load points.
Engineering Data:
E
=
29.
×
10
6
psi
l
1
= 15 ft
l
2
= 10 ft
Theoretical Solution:
(Lift-off occurs at point D only)
Point B:
Point D:
U y
= – 1.01 in
U y
=
+0.546 in
A
=
83.3 in
2
I z z
= 1000.0 in
4
I y y
=
334.0 in
4
P
1
= 40000 lb
P
2
=
10000 lb
CHAPTER 15
Verification and Validation
397
MSC.Nastran Results:
To compute the vertical displacement at the load points, the model shown in
generated using MSC.Patran. This model consisted of 13 CBEAM elements as well as two CGAP elements that were used to model the roller supports at points C and D. Since the CGAP elements had zero length, an additional coordinate frame, shown at the left end of the model, was used to define the orientation for both CGAP elements. In addition, both CGAP elements were provided a high closed stiffness, but no open stiffness. In this way the beam could lift-off the roller supports. Using this model, the following vertical displacements were calculated at both load points:
Table 15-1 Vertical Deflection of Beam with Lift-Off
Source
MSC.Nastran
Theory
%, Difference
U y
, Point B
-1.01
-1.01
0.0%
U y
, Point D
+0.546
+0.544
0.366%
The corresponding fringe plot that was made of the displacements with MSC.Patran is shown in
. Here the fringe plot for displacements has been superimposed upon an
exaggerated deformation plot. In addition, the maximum and minimum values for the vertical displacements are shown at the nodes where they occur. These values are clearly identical to the
MSC.Nastran results.
File(s):
<install_dir>/results_vv_files/prob012.bdf, prob012.op2
14
Basic Model with Loads and BCs
Figure 15-1 Model of Non-Linear Gap Problems with Lift-off.
398
PART 6
Results Postprocessing
14
Lift-off Deflection
Figure 15-2 Deflection Plot of Lift-off of Beam.
CHAPTER 15
Verification and Validation
399
Problem 14: Normal Modes, Point Masses and Linear Springs
Solution/Element Type:
MSC.Nastran, Normal Modes, Solution 103, CONM2 and CELAS1 Elements.
Reference:
Blevins, R.D., Formulas For Natural Frequency and Mode Shape, Kreiger Publishing Co., 1984, p. 50.
Problem Description:
Four equal masses are linked by five equal springs. Assuming that all motion is confined to the linear axis of the springs, determine the natural frequencies for the first four modes.
Engineering Data:
14
k
=
100
in
M
= 2.0
lb
–
in
sec
2
Theoretical Solution:
For a system consisting of four equal masses and five springs, the natural frequencies of and mode are given by the equations below. Substituting in the values for the mass and spring constants yields the following natural frequencies for the first four mode shapes:
f i
=
α
2
π
M
1/2
; i = 1, 2, 3, 4
α
=
2 sin
5
i
2
f
1
=
0.6955 Hz
f
2
=
1.3230 Hz
f
3
=
1.8209 Hz
f
4
=
2.1406 Hz
400
PART 6
Results Postprocessing
14
MSC.Nastran Results:
To compute the natural frequencies for the spring-mass system, the model shown in
was generated using MSC.Patran. The masses were modeled using CONM2 point mass elements while the springs were modeled with linear elastic CELAS1 elements. All motion was restricted to the x-, or axial, direction. The opposing ends of the model were fixed. The following results were computed:
Source
MSC.Nastran
Theory
%, Difference
Table 15-2 Natural Frequencies, Hertz
f
1
0.6955
0.6955
0.0%
f
2
1.3230
1.3230
0.0%
f
3
1.8209
1.8209
0.0%
f
4
2.1406
2.1406
0.0%
Due to the fact that all of the mode shapes merely involve horizontal displacements of the four masses, the mode shapes cannot be readily discerned by making combined fringe and deformation plots of the translational displacements associated with each eigenvector. Instead, vector plots were made of the translational displacement that were superimposed upon the deformed shape of the eigenvectors. In this way, the vectors would be drawn at the displaced position of each node, or mass. The eigenvectors and natural frequencies that were generated by
MSC.Patran for the first modes are plotted in
through
. Note that the natural frequencies recovered through MSC.Patran are identical to those obtained with
MSC.Nastran.
File(s):
<install_dir>/results_vv_files/prob014.bdf, prob014.op2
Basic Model
Figure 15-3 Spring and Mass Modal Model.
Mode 1, Freq=0.6955 Hz
Figure 15-4 Vector Plot of Mode 1.
Mode 2, Freq = 1.3230 Hz
Figure 15-5 Vector Plot of Mode 2.
CHAPTER 15
Verification and Validation
401
14
402
PART 6
Results Postprocessing
14
Mode 3, Freq = 1.8209 Hz
Figure 15-6 Vector Plot of Mode 3.
Mode 4, Freq = 2.1406 Hz
Figure 15-7 Vector Plot of Mode 4.
CHAPTER 15
Verification and Validation
403
Problem 15: Normal Modes, Shells and Cylindrical Coordinates
Solution/Element Type:
MSC.Nastran, Normal Modes, Solution 103, CTRIA3 Elements with Standard Formulation.
Reference:
Blevins, R.D., Formulas For Natural Frequency And Mode Shape, Kreiger Publishing Co., 1984, p.
240.
Problem Description:
Find the natural frequencies and mode shapes for a simply supported flat circular plate.
Engineering Data:
a = radius = 4.0 inches h = thickness = 0.25 inches
E = elastic modulus = 10
7
psi
ν
= poissons ratio = 0.3
γ
= weight per unit area = 6.5
×
10
–
5 lb-sec
2
/ in
3
14
0
1
2
3
Theoretical Solution:
For simply supported flat circular plate, the natural frequencies are given by the following expression:
Natural Frequency (hertz), f
i j
=
λ
2
------------
2
π
a
2
3
12
γ (
1 –
ν
2
)
1/2
; i = where for various values of i and j,
λ i j is given by:
j
4.977
29.76
74.20
138.3
0
Table 15-3
λ i j
j i
1
13.94
48.51
102.8
176.8
25.65
70.14
134.3
218.2
2
404
PART 6
Results Postprocessing
14
The natural frequencies for various modes are listed and shown below.
f
00
=
734.53 hz
i=0, j=0 i=0, j=1
f
10
=
2057.33 hz
f
20
=
3785.55 hz
f
01
=
4392.13 hz
f
11
= 7159.35 hz
f
02
=
10950.81 hz
i=1, j=0 i=2, j=0 i=0, j=2 i=1, j=1
MSC.Nastran Results:
To compute the mode shapes for the plate, the model shown in
to the cylindrical geometry, the model was meshed entirely with CTRIA3 elements which should provide accuracy better than a CQUAD4 element that is better suited for rectilinear geometry. In addition, the entire plate was modeled in order to provide better visualization of the modes. The following results were obtained.
Source
Theory
MSC.Nastran
%, Difference
Table 15-4 Natural Frequency, f
i j
(hertz)
f
00
f
10
f
20
f
01
f
11
f
02
734.53
2057.33
3785.55
4392.13
7159.35
10950.81
721.37
2034.82
3713.55
4238.06
6941.60
10125.20
-1.79% -1.09% -1.90% -3.51% -3.04% -7.54%
The corresponding combined fringe and deformation plots that were made for each of these modes are shown in
where the corresponding mode number and frequency have been clearly labeled.
File(s):
<install_dir>/results_vv_files/prob015.bdf, prob015.op2
Basic Model
CHAPTER 15
Verification and Validation
405
14
Figure 15-8 Basic Circular Membrane Model with h-Elements.
Mode i=0, j=0, Freq. = 721.37 Hz
Figure 15-9 Mode 1, f
00
, for Membrane h-Element Model.
406
PART 6
Results Postprocessing
14
Mode i=1, j=0, Freq. = 2034.8Hz
Figure 15-10 Mode 2, f
10
, for Membrane h-Element Model.
Mode i=2, j=0, Freq. =3.713.6Hz Hz
Figure 15-11 Mode 4, f
20
, for Membrane h-Element Model.
Mode i=0, j=1, Freq. =4238.1 Hz
Figure 15-12 Mode 6, f
01
, for Membrane h-Element Model.
CHAPTER 15
Verification and Validation
407
14
Mode i=1, j=1, Freq. =6941.6 Hz
Figure 15-13 Mode 9, f
11
, for Membrane h-Element Model.
408
PART 6
Results Postprocessing
14
Mode i=0, j=2, Freq. =10125 Hz
Figure 15-14 Mode 15, f
02
, for Membrane h-Element Model.
CHAPTER 15
Verification and Validation
409
Problem 16: Normal Modes, Pshells and Cylindrical Coordinates
Solution/Element Type:
MSC.Nastran, Normal Modes, Solution 103, CTRIA, P-Formulation
Reference:
Blevins, R.D., Formulas For Natural Frequency and Mode Shape, Kreiger Publishing Co,. 1984, p.
240.
Problem Description:
Problem 15: Normal Modes, Shells and Cylindrical Coordinates
which is to find the natural frequencies and mode shapes for a simply supported flat circular plate. In this instance, however, perform the calculation using cubic shell p-elements.
Theoretical Solution:
Problem 15: Normal Modes, Shells and Cylindrical Coordinates
MSC.Nastran Results:
To compute the modes for the plate, the model shown in
was generated using
MSC.Patran. Due to the curvilinear geometry and nature of the modes shapes, the model was meshed entirely with triangular shell elements. In this instance, all of the elements were cubic
TRIA13 p-elements. Due to the higher order of these elements, this permitted using a considerably sparser mesh than was used with simple linear TRIA3 elements in order to
properly capture the various modes. A sparser mesh than what is shown in
found to only give reasonably accurate results for only the very lowest modes. The lack of an appropriate number of degrees of freedom necessarily precluded capturing some of the higher modes which typically exhibit considerably more complex shapes.
The following natural frequencies were calculated for some of the various modes.
f
00
=
726.71 hz
f
10
= 2037.80 hz
f
20
=
3736.80 hz
f
01
= 4377.78 hz
f
11
=
7259.80 hz
f
02
= 11178.31 hz
Source
Theory
MSC.Nastran
%, Difference
Table 15-5 Natural Frequency,
f
i j
(hertz)
f
00
f
10
f
20
f
01
f
11
f
02
734.53
2057.33
3785.55
4392.13
7159.35
10950.81
726.71
2037.80
3736.80
4377.78
7259.80
11178.31
-1.06% 0.95% -1.29% -0.33% 1.40% 2.08%
The corresponding combined fringe and deformation plots that were made with MSC.Patran for each of these modes are shown in
and frequency have been clearly labeled. A comparison of these figures with the figures of
Problem 15: Normal Modes, Shells and Cylindrical Coordinates
the predicted mode shapes are being accurately predicted by MSC.Nastran and displayed with
14
410
PART 6
Results Postprocessing
MSC.Patran. In addition, it is interesting to note that the use of higher order pshell elements gives comparable accuracy for the first couple of primary modes but gives noticeably more accurate results for the higher order modes, the error being typically about one-fourth or less.
File(s):
<install_dir>/results_vv_files/prob016.bdf, prob016.op2
14
Basic p-Element Model
Figure 15-15 Basic p-Element Membrane Model.
MODE i=0, j=0, Freq.=726.71 Hz
Figure 15-16 Mode 1, f
00
, of p-Element Membrane Model.
MODE i=1, j=0, Freq.=2037.8 Hz
Figure 15-17 Mode 2, f
10
, of p-Element Membrane Model.
CHAPTER 15
Verification and Validation
411
14
MODE i=2, j=0, Freq.=3736.8 Hz
Figure 15-18 Mode 4, f
20
, of p-Element Membrane Model.
412
PART 6
Results Postprocessing
14
MODE i=0, j=1, Freq.=4377.8 Hz
Figure 15-19 Mode 6, f
01
, of p-Element Membrane Model.
MODE i=1, j=1, Freq.=7259.8 Hz
Figure 15-20 Mode 9, f
11
, for Membrane p-Element Model.
CHAPTER 15
Verification and Validation
413
14
MODE i=0, j=2, Freq.=11178 Hz
Figure 15-21 Mode 15, f
02
, of p-Element Membrane Model.
414
PART 6
Results Postprocessing
14
Problem 17: Buckling, shells and Cylindrical Coordinates
Solution/Element Type:
MSC.Nastran, Buckling, Solution 105, CTRIA3, CQUAD4 Elements with Standard Formulation.
Reference:
Roark, R.J., and Young, W.C., Formulas For Stress and Strain, 5th ed., McGraw-Hill, Book
Company, 1975, p. 556.
Problem Description:
Find the critical buckling pressure for a thin wailed cylinder with closed ends subjected to a uniform external pressure both laterally and longitudinally. Assume the endcaps and cylinder have the same thickness and that the ends are held circular.
Engineering Data:
E
= elastic modulus = 1
×
10
7
psi
ν
= Poissons Ratio = .33
l
= length = 20 inches
r
= radius = 5.0 inches
t
= thickness = .125 inches
q
= pressure
Theoretical Solution:
For a thin walled cylinder with closed ends subjected to a uniform external pressure both axially and longitudinally, the critical buckling pressure is given by the following expression:
q c r i t
=
E
----------------------------
1 +
2
--
r t
------
nl r
2
n
2
1
+
nl
π
r
2 2
+
2
t
2
12r
2
(
1
–
ν
2
)
+
π
r
2 2
Upon substitution of the engineering design parameters into the preceding equation, it can be shown that the minimum buckling pressure corresponds to a three lobed buckling mode shape.
This occurs at a critical pressure equal to:
q c r i t
= 256.23 psi
.
CHAPTER 15
Verification and Validation
415
MSC.Nastran Results:
To compute the critical buckling pressure for the cylinder, the model shown in
generated using MSC.Patran. The lateral sides of the cylinder were meshed with CQUAD4 elements while owing to the curvilinear geometry, the endcaps were meshed with CTRIA3 elements to maximize accuracy. Due to symmetry, only half of the cylinder was modeled with the appropriate symmetry boundary conditions being applied along the free edges. Additional symmetry boundary conditions were applied along the midplane of the cylinder. Also, to prevent recovery of any modes associated with buckling of just the endcaps, the center of each cap was restrained against any motion in either the radial, tangential or axial directions.
A buckling calculation was performed using MSC.Nastran. The critical buckling pressure was predicted to be:
Table 15-6 Critical Buckling Pressure
Theory
MSC.Nastran
%, Difference
256.23psi
270.18psi
5.44%
The corresponding mode shape was plotted with MSC.Patran and is shown in
The mode shape clearly shows two distinct lobes present on the half of the cylinder that was modeled, with an additional lobe present on the other half that was not included due to symmetry.
File(s):
<install_dir>/results_vv_files/prob017.bdf, prob017.op2
14
Basic Model with Loads and BCs
Figure 15-22 Cylinder Buckling Model with Loads and BCs.
416
PART 6
Results Postprocessing
First Buckling Mode
Critical Pressure = 270.18 PSI
14
Figure 15-23 Three Lobed Mode Corresponding to Critical Pressure.
CHAPTER 15
Verification and Validation
417
Problem 18: Buckling, Flat Plates
Solution/Element Type:
MSC.Nastran, Buckling, Solution 105, CQUAD4 with Standard Formulation.
Reference:
Roark, R. J., and Young, W. C., Formulas For Stress and Strain, 5th ed., McGraw-Hill Book
Company, 1975, p. 551.
Problem Description:
A simply supported flat rectangular plate is subjected to a uniform compressive edge load. Find the critical buckling edge load and corresponding buckling mode shape.
Engineering Data:
E
= elastic modulud = 1
×
10
7
psi
ν
= Poissons Ratio = .33
t
= thickness = .1 inches
a
= length = 16 inches
b
= width = 4 inches
14
Theoretical Solution:
For a simply supported plate subjected to edge pressures
σ
x
and , the critical edge pressure required to induce buckling is given by:
σ
y
σ
m
2
2
σ
a
+
2
b
2
=
0.823
1
–
ν
2
2
a
2
2
+
2
-----
b
2
Here m and n signify the number of half-waves in the buckled plate in the x and y directions respectively. Assuming that:
σ
=
σ
=
σ
* and:
m
=
n
=
1 yields:
σ
*
= 0.823
1 –
ν
2
2
a
2
+
b
2
Substitution of the design parameters for the plate yields a critical edge pressure of:
σ
*
=
6133.13 psi which corresponds to a distributed edge load of 613.313 lbs / inch.
418
PART 6
Results Postprocessing
14
MSC.Nastran Results:
To compute the critical buckling load and mode shape for the plate, the model shown in
was created using MSC.Patran. Due to symmetry, only one-fourth of the plate was
modeled with the appropriate boundary conditions being applied along the planes of symmetry.
In addition to further enforce recovery of only the lowest mode, additional boundary conditions were imposed so that there were no surface rotations about axes located in either plane of symmetry. This would ensure that only symmetrical mode shapes were calculated. Lastly, compressive edge pressures were modeled as distributed edge loads equal to the edge pressure multiplied by the plate thickness. Using this model, MSC.Nastran calculated the critical edge pressure to be:
Theory
Table 15-7 Critical Edge Pressure
MSC.Nastran
%, Difference
σ
*
=
6133.13 psi
σ
*
= 6133.25 psi
0.002%
The corresponding buckling mode shape that was plotted using MSC.Patran is shown in
. The mode shape plot clearly reveals the presence of a half-sine wave in either the
x or y directions, which would correspond to m = n = 1.
File(s):
<install_dir>/results_vv_files/prob018.bdf, prob018.op2
Basic Model with Loads and BCs
Figure 15-24 Plate Buckling Model with Load and BCs.
First Buckling Mode
CHAPTER 15
Verification and Validation
419
14
Figure 15-25 Buckling Mode Shape of Plate due to Critical Pressure.
420
PART 6
Results Postprocessing
14
Problem 19: Direct Transient Response, Solids and Cylindrical
Coordinates
Solution Type:
Direct Linear Transient Response, Solution 109
Element Type:
CHEX8, Standard Formulation
Reference:
Crandall, S. H., Dahl, N.C., and Lardner, T.J., An Introduction to the Mechanics of Solids, 2nd ed.,
Mc-Graw Hill Book Company, 1972, pp. 293-297.
Problem Description:
A thick walled cylinder is subjected to a sudden internal pressure of 10 psi. Find the peak radial displacement in the cylinder due to the sudden application of the pressure.
Engineering Data:
r i
= 6.0 inches r
0
= 12.0 inches h = 8.0 inches
E = 30.0 x 10
6 psi
ρ
=
.28 lbs / in
3
ν
=
0.0
P = 10.0 psi
ri ro h
Theoretical Results:
For a single degree-of-freedom system, an instantaneously applied load will give a maximum displacement that is twice the static displacement at the same applied loading.
MSC.Nastran Results:
To determine the transient response of the cylinder, the model shown in
generated using MSC.Patran. Due to symmetry, only a 15 degree sector of the cylinder was modeled with the appropriate axisymmetric boundary conditions applied to the lateral faces of the model. The model was meshed entirely with CHEX8 solid elements using a standard formulation.
For the purposes of this analysis, the pressure was applied in an instantaneous manner as shown below. Several time steps of zero load were input to ensure simulation of a sudden step function in the loading. The integration time step was chosen to be 1.0 microsecond. To prevent numerical instability, the applied loading was ramped over a single time step. Approximately three cycles
CHAPTER 15
Verification and Validation
421
of the response were simulated and structural damping was neglected with the radial displacement being recovered at three radial positions situated at the inner diameter, midway through and at the outer diameter of the cylinder.
1.0
Force
Multiplier
1
14
0
1 2 3 4 5 6
7
8 9
10 t (microseconds)
Using the same model, a static analysis was performed with a constant internal pressure of 10.0 psi. The results for both the static and transient analysis are summarized below.
Position
r i r me a n r
0
Table 15-8 Transient vs. Static Results
Static
Displacement
(
x
10
– 6
)
3.325737
2.773202
2.662867
Peak Transient
Displacement
(
x
10
– 6
)
6.534348
5.534836
5.322965
Ratio Transient/Static
1.965
1.996
1.999
An XY Plot that was generated by MSC.Patran of the transient radial displacement at inner, mean, and outer radius is shown in
. In this figure nodes 120, 123 and 126
correspond to the inner, mean and outer radius, respectively. The results clearly show the expected oscillatory behavior characteristic of an undamped response. The corresponding static results are shown in
where the radial displacement has been plotted against
radius.
A fringe plot of the static radial displacements is shown in
xyplots clearly show peak values that agree with he preceding MSC.Nastran results.
File(s):
<install_dir>/results_vv_files/prob019_T.bdf, prob019_T.op2, prob019_S.bdf, prob019_S.op2
422
PART 6
Results Postprocessing
Basic Model with Loads and BCs
14
Figure 15-26 Transient Dynamic Model of Cylinder.
Corresponding
Static
Displacements
Figure 15-27 Corresponding Static Results of Displacement.
CHAPTER 15
Verification and Validation
423
14
Figure 15-28 Displacement Responses at Various Nodes.
Figure 15-29 Corresponding Static Displacements Across Thickness.
424
PART 6
Results Postprocessing
14
Problem 20:Modal Transient Response with Guyan Reduction and
Bars, Springs, Concentrated Masses and Rigid Body Elements
Solution/Element Type:
MSC.Nastran, Modal Transient Response, Solution 112, CBAR, CONM2, CMASS1, CELAS1,
RBE2.
Reference:
MSC.Nastran Demonstration Problem Manual, Version 65
Problem Description:
The transient response is required of a two dimensional truss mounted on an elastic foundation and subjected to a time dependent base excitation. The truss is shown below and consists of bars of varying cross-section with localized concentrated masses. The horizontal acceleration that is applied to the base is shown plotted in
.
X B
13
9
16
11
18
15
8
6
4 5
17
12
10
14
7
2 3
1
CHAPTER 15
Verification and Validation
425
Engineering Data:
Table 15-9 Bar Properties Foundation Stiffness
Bar ID
1
2 through 5
6,7,13,14
8
6 through 12
15, 18
16, 17
19, 20
Area
36.91371
30.63052
266.83900
30.63052
24.34734
147.65490
162.57740
537.21123
I1
2549.353
1456.865
47701.650
1456.865
731.942
40789.650
24234.200
22965.830
Table 15-10 Foundation Stiffness
Direction
Vertically
Horizontally
Rotationally
Stiffness
23.0 x 10
5
1.0 x 10
5
15.0 x 10
9
Table 15-11 Concentrated Masses
Location (Point ID)
15, Horizontal
15, Vertical
15, Rotational
3, 4, 6, 7
5, 8
9, 10
11, 12
Mass
8.0 x 10
9
8.0 x 10
9
4.0 x 10
15
388.1988
25.8799
1035.197
2070.393
Theoretical Solution:
For this particular problem there exists no simple closed form solution. The only real means of ascertaining the accuracy of a MSC.Nastran analysis model is to ensure that the base acceleration matches the intended profile of the applied excitation. This is a basic check that should always be performed, especially when using the large mass method to simulate an enforced base motion.
14
426
PART 6
Results Postprocessing
14
MSC.Nastran Results:
To calculate the transient response for the truss, the model shown in
generated using MSC.Patran. The model was comprised of simple CBAR elements and CONM2 elements that were used to model any localized masses, with the exception of the base point (i.e.,
Node 15). To model the base, three large grounded scalar mass CMASS1 elements were used, one each for the horizontal, vertical and rotational directions. The magnitude of these masses were chosen to be approximately 10
9
times as great as the mass of the truss. By doing so, this would ensure that the large mass of the base would dominate so that the intended base excitation was properly applied to the entire truss. A single RBE2 rigid body element was used to attach the base node to the ends of the CELAS1 elements that were used to model the elastic foundation.
In performing the analysis, the modal transient method was used along with automated Guyan reduction. The transient response was based upon the first 30 modes which spanned a frequency range that extended to approximately 100 hertz. This was deemed more than acceptable, given the periodicity of the applied base acceleration profile. In addition, it was assumed that throughout this entire frequency range, the truss was 10 percent critically damped.
The resultant acceleration profile that was predicted by MSC.Nastran at the base point is shown
. Here the horizontal acceleration at node 15 has been plotted versus time
using the results xyplot utility of MSC.Patran. It can clearly be seen that the acceleration at Node
15 closely matches the intended base excitation which was previously shown in
The acceleration at other selected nodes on the model are shown plotted in
acceleration profiles appear to show the correct response. Namely, the occurrence of any localized peaks in the base acceleration are matched by localized peaks in the acceleration of the truss. Similarly, the magnitude of the bar forces and stress response plots, shown in
, exhibit the same behavior.
File(s):
<install_dir>/results_vv_files/prob020.bdf, prob020.op2
Figure 15-30 Horizontal Acceleration Applied to Truss.
Basic Model of Truss with Boundary Conditions
Figure 15-31 Basic Model of 2D-Truss Structure.
CHAPTER 15
Verification and Validation
427
14
Figure 15-32 Horizontal Acceleration Profile at Base (Node 15).
428
PART 6
Results Postprocessing
14
Figure 15-33 Horizontal Acceleration at Selected Points of 2D-Truss.
Figure 15-34 Bar Force Responses at Selected Points in 2D-Truss.
CHAPTER 15
Verification and Validation
429
14
Figure 15-35 Stress Responses at Selected Points in 2D-Truss.
430
PART 6
Results Postprocessing
14
Problem 21: Direct Nonlinear Transient, Stress Wave Propagation with 1D Elements
Solution/Element Type:
MSC.Nastran, Direct Nonlinear Transient, Solution 129, CROD Elements
Reference:
Timoshenko, S., and Goodier, J. N., Theory of Elasticity, 2nd ed., McGraw-Hill Book Co., 1951, pp.
492-496.
Juvinall, R.C., Engineering Consideration of Stress, Strain and Strength, McGraw-Hill Book Co.,
1967, pp. 185-188.
Problem Description:
A rod of uniform cross section is fixed at one end and a constant force is suddenly applied to its free end. A stress wave results that propagates along the length of the rod. Determine the stress history at both the free and fixed ends of the rod as well as the displacement history at the free end.
Engineering Data:
L = rod length = 100.0 m
E = elastic modulus = 103 N/m
2
ρ
= mass density = 0.1 kg / m
3
A = cross-sectional area of the rod = 1.0 m
2
ν
=
Poissons Ratio = 0.3
c
=
E
/
ρ
=
100.0 m/sec = stress wave velocity
Theoretical Solution:
Due to the constant force, F, applied at the free end of the rod, the stress at the free end remains constant and is simply equal to
σ
= –
A
= –
1000.0 N/m
2
CHAPTER 15
Verification and Validation
431
Before the stress wave first reaches the fixed end, the stress at the fixed end is zero. As soon as the stress wave arrives at the fixed end, it is reflected and produces a stress equal to
2
σ
at the fixed end. The stress remains unchanged until the wave front returns to this point. The compressive wave leaves the fixed end and upon reaching the free end it is once again reflected, but this time as a tensile wave. When this tensile wave arrives at the fixed end and is reflected, the stress at the fixed end becomes zero. This zero stress state will again remain unchanged for another complete cycle of the stress wave motion.
The displacement time history at the free end can be expressed as
=
∫
L
0
σ (
x t
)
Or, expressing u(t) separately for each time interval
,
=
–
FL t
2
AE
≤ ≤
u t
(
= 2
)
+
–
FL
AE
(
– 2
)
for 2
t
4 etc.
Thus, the displacement at the free end is a linear function of time during each interval it takes the stress wave to completely traverse the rod.
MSC.Nastran Results:
To determine the stress and displacement history at the opposing ends of the rod, the model shown in
was generated using MSC.Patran. The model consisted of 20 CROD
elements. One end was fixed while the remainder of the rod was constrained to motion in the x, or axial, direction only. The upper bound stability limit for the integration time increment was determined by:
∆
t
=
(
n
1
)
m ax
where
( ϖ
n
)
is the highest natural frequency in cycles per second of all of the modes of interest
ma x
in the model. In this instance, this would mandate that modal frequencies be at least greater than the frequency associated with one complete cycle for the stress wave to completely traverse the rod, or 0.5 cycles per second. For the purposes of this analysis, an integration time increment of
0.025 seconds was used. In addition, a slight amount of damping was introduced to reduce the overall occurrence of any oscillations in the solution.
Stress history plots that were made with MSC.Patran of the MSC.Nastran results are shown in
for the fixed and free ends of the rod, respectively. The displacement history at the free end of the rod is shown plotted in
presence of the damping, the results do exhibit some slight oscillations, especially whenever a
14
432
PART 6
Results Postprocessing
14
stress wave is reflected as well as upon initial application of the loading. However, these oscillations are rapidly attenuated. Overall, the results demonstrate the correct periodicity of the stress and displacement at both the fixed and free ends of the rod.
Table 15-12 Maximum Displacement, t=2
Seconds
Theory
MSC.Nastran
%, Difference
200.00 m
200.98 m
0.49%
Table 15-13 Maximum Stress at Fixed End,
1<t<3 Seconds
Theory
MSC.Nastran
%, Difference
–
2000. N / m
2
–
2264.6 N / m
2
13.23%
File(s):
<install_dir>/results_vv_files/prob021.bdf, prob021.op2
Figure 15-36 Basic CROD Model to Investigate Stress Wave.
CHAPTER 15
Verification and Validation
433
14
Figure 15-37 Stress History Plot at Element 20, the Free End.
Figure 15-38 Stress History Plot at Element 1, the Fixed End.
434
PART 6
Results Postprocessing
14
Figure 15-39 Free End Displacement of CROD Model.
CHAPTER 15
Verification and Validation
435
Problem 22: Direct Nonlinear Transient, Impact with 1D,
Concentrated Mass and Gap Elements
Solution/Element Type:
MSC.Nastran, Direct Nonlinear Transient, Solution 129, CROD, CGAP, CONM2 Elements.
Reference:
Timoshenko, S., and Goodier, J.N., Theory of Elasticity, 2nd ed., McGraw-Hill Book Co., 1951, pp.
497-504
April 1986 Application Note, Application Manual Section 5.
Problem Description:
of the mass prior to impact. Consider the mass of the body to be infinitely rigid and the velocity of stress and displacement at the free end of the rod as well as the duration of the impact and the maximum stress in the rod.
Engineering Data:
L = rod length = 100.0 m
A = cross-sectional of the rod = 1.0 m
2
ν
=
Poissons Ratio = .3
E = elastic modulus = 10
3
N / m
2
ρ
=
0.1 kg / m
3
M = moving mass = 10.0 kg m = rod mass =
ρ
AL
= 10.0 kg v
0
= –
0.1 m / sec
14
A
L vo
Rod mass = m
M
436
PART 6
Results Postprocessing
14
Theoretical Solution
At the instant of impact, an initial compressive stress is generated at the free end of the rod equal to:
σ
0
= v
0
E
ρ or upon substitution:
σ
0
= – 1.0 N / m
2
After impact, the resistance of the bar will cause the velocity of the moving body to decrease and hence the pressure on the bar will decrease as well, causing a reduction in the compressive stress in the bar. Thus, there exists a compressive wave characterized by a decreasing compressive stress traveling along the length of the bar. The change in compressive stress with time can easily be determined from the equation of motion of the body. Letting denote the variable compressive stress at the free end of the bar and v the variable velocity of the body yields:
M dv
σ
dt
+ =
0 or upon substituting
ν
=
E
ρ yields:
E
ρ
d
σ
dt
+
σ
=
0 from which
σ
=
σ
0
e
–
t E
ρ
M
This equation is only valid so long as
t
<
2l / E
ρ
, or
t
<
2
seconds. At t = 2 seconds, the compressive wave with an intensity of
σ
0
returns to the free end of the bar, which is still in contact with the body. The velocity of the body cannot change suddenly. As a consequence, the stress wave will be reflected from the end of the bar, resulting in an immediate increase in the compressive stress to
2
σ
0
. This sudden change in compressive stress occurs during impact at the end of every two second interval. However, during every subsequent interval, there will be an increasing number of stress waves either moving away or toward the struck end of the rod. The compressive stress at the free end of the rod at any instant will simply be the sum of the stress induced by the reflected waves produced during that particular interval with the stress produced by the returning waves from the previous interval. The actual peak stress produced in the rod throughout impact will occur in a different interval depending upon the ratio of the mass of the rod to the mass of the body. For the case
α
= 1
, the max stress occurs at t = 2 seconds and is equal to
2
σ
0
.
CHAPTER 15
Verification and Validation
437
The instant when the stress at the free end of the rod becomes zero indicates the end of impact.
In general the duration of the impact increases as decreases. Calculations of Saint-Venant give the following values for impact duration:
α
=
1/6
Duration
7.419
1/4
5.900
1/2
4.708
1
3.068
MSC.Nastran Results:
To determine stress and displacement history at the free end of the rod, the model shown in
was generated using MSC.Patran. The model consisted of 20 CROD elements. The
end of one CROD element was completely restrained while the remainder were constrained to motion in the x, or axial, direction only. The mass was modeled with a CONM2 concentrated mass element which was connected to the free end of the rod with a gap element having a zero initial opening. An initial velocity of v
0
= –
0.1 m/sec
was specified for both the CONM2 and the node situated at the free end of the rod. An integration time step of 0.025 seconds was chosen and a small damping of 0.4% was introduced to reduce any high frequency oscillations in the solution.
The MSC.Nastran results are shown in
and
and displacement history at the free end of the rod were plotted using MSC.Patran. Also shown
is the displacement history of the mass, designated as Node 22. The results show
the expected behavior; namely, an initial compressive stress of
–
1.0 N / m
2
that rapidly decays until 2 seconds at which time it immediately doubles and then decays to a value of zero. The time at which the stress reaches zero also correlates in
longer moving in unison, which signifies the end of impact.
Source
Theory
MSC.Nastran
%, Difference
Table 15-14 Rod Impact Results
Max Stress
(N / m
2
)
-2.00
-1.84
-8.0%
Impact Duration (sec)
3.068
3.075
0.23%
File(s):
<install_dir>/results_vv_files/prob022.bdf, prob022.op2
14
438
PART 6
Results Postprocessing
14
Basic Model with Boundary Conditions
Figure 15-40 Basic Model of Impact Analysis.
Figure 15-41 Free End Stress Response of Impact Model.
CHAPTER 15
Verification and Validation
439
14
Figure 15-42 Rod End and Mass Displacement Responses.
440
PART 6
Results Postprocessing
14
Problem 23: Direct Frequency Response, Eccentric Rotating Mass with Variable Damping
Solution/Element Type:
MSC.Nastran, Direct Frequency Response, Solution 108, CBAR, CELAS1, CDAMP1, and
CONM2 Elements.
Reference:
Thomson, W. T., Theory of Vibration with Applications, Prentice-Hall, Inc., 1972, pp. 45-52.
Problem Description:
A spring mass system is constrained to move in the vertical direction and is excited by a rotating machine that is unbalanced as shown below. The unbalance is represented by an eccentric mass, m, with eccentricity, e, which is rotating at an angular velocity, . Determine the undamped resonant frequency as well as the amplitude at this frequency when the damping is varied.
Engineering Data:
k = spring constant = 1000.0 lbf / inch c = 2.5, 10.0 or 30.0 lbf-sec / inch e = 0.1 inch m = eccentric mass = .0633 lb-sec
2
/ inch
M = total mass = .25 lb-sec
2
/ inch where:
m e
=
2
------
n
---------------------------------------------------------------------
1 –
ω
ω
n
2 2
+ 2 ------
n
2
c c
=
2m
ω
n
= critical damping factor
ζ
=
c c
= critical damping ratio
CHAPTER 15
Verification and Validation
441
The resonant amplitude is then given by
For c = 2.5,
For c = 10.0,
For c = 30.0,
ζ
=
0.07906
ζ
=
0.31622
ζ
=
0.94868
X
=
-------
2
ζ
X
=
0.1602036 inches
X
=
0.0400509 inches
X
=
0.0133503 inches
MSC.Nastran Results:
To model the eccentrically rotating mass system, the model shown in
generated using MSC.Patran. To improve visualization, the nonrotating mass was modeled as a rod using two CBAR elements. The rod had a total mass equal to that of the nonrotating mass
(M - m) and the eccentric mass m, or 0.25 lb-sec
2
/inch. The ends of the rod were constrained to move in the y, or vertical, direction only. The ends of the rod were attached to grounded springs, each with a stiffness of 500 lbs/inch. The center of the rod was attached to a grounded damper.
In addition, at the center of the rod, the force due to the rotation of the eccentric mass was applied. A plot of the applied force versus frequency is shown in
Using this model, a frequency response analysis was performed whereby the frequency and rotational loading was varied over a range of 0 to 30 hertz. The displacement at the center of the
rod was recovered and is shown plotted in
. Here the MSC.Nastran results have been plotted with the aid of MSC.Patran for each of the damping ratios that were examined. The magnitude of the complex results is plotted. The results clearly reveal the presence of a resonant spike occurring at about 10 hertz that becomes rapidly attenuated as the damping is increased.
At the highest damping level, a critically damped response is highly evident that is characterized by the absence of any amplification in the displacement at the resonant frequency.
Source
Theory
MSC.Nastran
%, Difference
Table 15-15 Amplitude at Resonant Frequency
ζ
=
0.0790569
0.160236
0.1586090
-0.995%
ζ
=
0.0400509
0.0400509
0.0397802
-0.676%
ζ
=
0.948683
0.0133503
0.0132626
-0.657%
File(s):
<install_dir>/results_vv_files/prob023_1.bdf, prob023_1.op2, prob023_2.bdf, prob023_2.op2, prob023_3.bdf, prob023_3.op2
14
442
PART 6
Results Postprocessing
14
Figure 15-43 Basic Model of Direct Frequency Response Analysis.
Figure 15-44 Applied Force versus Frequency.
Figure 15-45 Amplitude Displacements at Center of Rod.
CHAPTER 15
Verification and Validation
443
14
444
PART 6
Results Postprocessing
14
Problem 24: Modal Frequency Response, Enforced Base Motion with Modal Damping and Rigid Body Elements
Solution/Element Type:
MSC.NastranModal Frequency Response, Solution 111, CQUAD4, CELAS1, CONM2, and RBE2
Elements.
Reference:
Thomson, W.T., Theory of Vibration with Applications, Prentice-Hall, Inc., 1972, pp. 45-49.
Problem Description:
A long thin cantilevered plate has a concentrated mass suspended from its free end by two parallel springs. The base of the plate is excited by a sinusoidal excitation producing a peak unit acceleration. Find the resultant acceleration response of the suspended mass and the tip of the plate over a frequency range of zero to 100 hertz.
Engineering Data:
l = 12.0 inches w = 2.0 inches t = 0.5 inches k = 50 lbf / inch
E
= elastic modulus = 10
7
psi
ν
=
Poissons ratio = .33
ρ
= mass density of plate = 0.026 lbf-sec
2
/ inch
4
m
= end mass = 0.5 lbf-sec
2
/ inch
ζ
= critial damping ratio = 0.1
k m t w
Theoretical Solution:
For the cantilevered plate and suspended mass, the application of a sinusoidal base excitation will produce a resonant spike at each of the mode shapes associated with the end mass and with the tip of the plate. The amplitude induced at resonance will be a function of the amount of damping present. To determine where the expected resonant points occur, it is first necessary to estimate the natural frequencies for the end mass and plate.
First consider the end mass. This mass is suspended by two parallel springs whose total combined stiffness is simply the sum of the two. However, this combined spring is in series with another spring determined by the stiffness of the plate. For a cantilevered plate, the spring stiffness is given by:
k pl a t e
=
l
3
CHAPTER 15
Verification and Validation
445
Substituting the assumed engineering data gives:
k p la t e
=
361.69 lbf / inch
The total effective combined stiffness of the plate and the end springs is given by
k t o t al
=
2k
2k
×
+
k k pl a t e p l a t e
=
78.34 lbf / inch
The resonant frequency for the end mass then becomes:
f ma s s
=
For the cantilevered plate, the resonant frequencies are given by
f i
=
λ
-----------
2
π
l
2
----------------
m p l a t e
1/2 where
m p l a t e
is the mass per unit length.
For the first two modes:
λ
1
= 1.875
λ
2
= 4.694
This gives for the plate:
m
=
1.993 hertz
f
1
= 10.99 hertz
f
2
= 68.89 hertz
Since there exists a single resonant frequency associated with the motion of the end mass that lies within the frequency range of interest, the application of a unit base acceleration should cause a resonant response only at frequencies in the vicinity of 1.933 hertz. In contrast, for a point situated on the end of the plate, two additional resonant spikes will occur at frequencies near
10.99 hertz and 68.89 hertz.
For a harmonically excited damped oscillator, the width of the resonant spike is expressed by the factor Q which is defined as:
Q
=
------
2
ζ
=
ω
n
∆ω
=
ω
1
ω
n
–
2 where
ω
1
and
ω
2
refer to those frequencies above and below approximately 70 percent of the response that occurs when
ω
n
where the response is
ω
=
ω
n
. These frequencies are referred to as the half power points. If the damping remains fixed over the entire frequency range of interest, then the bandwidth about the resonant points must be noticeably greater at the higher natural frequencies. Thus, a very narrow band response should be observed at low frequencies becoming increasingly broadband at the natural frequencies associated with the higher modes.
MSC.Nastran Results
To determine the frequency response of the system, the model shown in
was generated using MSC.Patran. The plate was modeled using standard CQUAD4 elements. The end mass was modeled using a lumped mass CONM2 element which was attached to the plate with two CELAS1 linear spring elements. To simulate the base, the other end of the plate was
14
446
PART 6
Results Postprocessing
14
attached to an RBE2 rigid body element. At the independent node for the RBE2 element, a large concentrated mass was placed and excited by a force of sufficient magnitude to cause a unit acceleration throughout the frequency range of interest. The magnitude of the mass for the base was chosen to be 10
6
times as great as the entire mass of the plate and suspended end mass. This would ensure that the inertia of the base would dominate and impose the desired enforced motion. For the purpose of this analysis, the model was purposely constrained to prevent any lateral motion.
Before determining the frequency response of the plate-mass system, a modal analysis was performed to determine the natural frequencies and corresponding mode shapes. The first three predicted modes were plotted using MSC.Patran and are shown in
through
. Also displayed in these figures are the corresponding natural frequencies.
Examination of these figures shows excellent agreement with the predicted modes. The first mode is predominately associated with motion of the end mass, whereas the higher modes mainly entail excitation of the plate. On the basis of the modal analysis, a frequency response analysis should exhibit a resonant peak in the acceleration occurring 2.0054, 12.84 and 71.134 hertz.
A subsequent frequency response analysis was performed with the preceding model using the modal method. For the purpose of this analysis, only the first five modes were retained, which included frequencies up to 195 hertz. This was deemed satisfactory since the maximum frequency of interest was only 100 hertz. The accelerations were recovered at the base, the suspended end mass and at the tip of the plate. These accelerations are shown plotted in
where the magnitude of the complex result has been plotted. The resultant
accelerations show the correct behavior. The end mass shows a single resonant spike at the first mode, or approximately 2 hertz, whereas the plate tip shows three distinct resonance points occurring at each of the three natural frequencies that were previously calculated. In addition, the base shows a uniform unit acceleration over the entire frequency band, clearly indicating that a sufficiently large mass was chosen to obtain the desired enforced motion. Lastly, the resonant spikes for the plate tip shows an increasingly broadband behavior that would be consistent with a constant Q, or damped system.
For the problem at hand, there exists no rigorous closed form solution. The presence of the elastically suspended mass on a cantilevered plate creates a multi degree of freedom system.
Closed form solutions only exist for single degree of freedom damped oscillators. Nevertheless, the estimated modes show the correct mode shapes and are occurring at approximately the expected natural frequencies. In addition, resonant peaks are occurring in the vicinity of the predicted natural frequencies, with an increasing broadband response at the higher modes that would be indicative of uniform modal damping.
File(s):
<install_dir>/results_vv_files/prob024_1.bdf, prob024_1.op2, prob024_2.bdf, prob024_2.op2
Figure 15-46 Model of Beam with Suspended Mass.
MODE 1, Freq.=2.0054 Hz
CHAPTER 15
Verification and Validation
447
14
Deflection 1.409772 @NODE 40
Figure 15-47 First Mode Shape of Beam, Freq=2.0054 Hz.
448
PART 6
Results Postprocessing
14
MODE 2 Freq.=12.84 Hz
Figure 15-48 Second Mode Shape of Beam, Freq = 12.84 Hz.
MODE3, Freq.=71.134 Hz
Figure 15-49 Third Mode Shape of Beam, Freq = 71.134 Hz.
CHAPTER 15
Verification and Validation
449
14
Figure 15-50 Acceleration Responses of Plate Tip, End Mass, and Base.
450
PART 6
Results Postprocessing
14
Problem 25:Modal Frequency Response, Enforced Base Motion with Modal Damping and Shell P-Elements
Solution/Element Type:
MSC.Nastran, Modal Frequency Response, Solution 111, CQUAD16, CELAS1, CONM2
Reference:
Thomson, W.T., Theory of Vibration with Applications, Prentice-Hall, Inc., 1972, pp. 41, 108, 158.
Problem Description
Problem 24: Modal Frequency Response, Enforced Base Motion with
Modal Damping and Rigid Body Elements
(p. 444) with the exception that cubic QUAD16
pshell elements were used to model the plate. See this problem for a description of the model and all relevant engineering data.
Theoretical Solution
MSC.Nastran Results:
To determine the frequency response of the suspended end mass and the tip of the plate, the
was generated using MSC.Patran. In this instance, the plate was
modeled using two cubic QUAD16 elements. The suspended mass was attached to the end of the plate using CELAS1 elements. Since RBE2 elements are not functional with p-elements, this necessitated that two large masses be attached directly to the corners at the base of the plate. At the site of the large masses, two sinusoidal forces were applied that were of sufficient magnitude to impart a unit acceleration throughout the entire frequency range of interest, or zero to 100 hertz. As before, base masses were chosen that were on the order of 10
6 times the mass of the plate and the suspended end mass. This would ensure that the desired enforced motion was being imparted at the base of the plate. In addition, a constant 10% critical modal damping was assumed.
Using the preceding model, a modal analysis was performed to determine all of the relevant modes that existed in the frequency range between zero and 100 hertz. The results of this analysis showed the existence of three distinct modes at the following frequencies:
Table 15-16 Predicted Natural Frequencies
Mode Number
1
2
3
Natural Frequency (Hertz)
2.009
12.984
72.613
The corresponding mode shapes were identical to those shown in
Problem 24: Modal Frequency Response, Enforced Base Motion with
Modal Damping and Rigid Body Elements
(p. 444). In addition, the predicted natural
frequencies closely matched those that were obtained with linear CQUAD4 elements, which were 2.0054, 12.840 and 71.134 hertz. The results of a frequency response analysis are shown in
CHAPTER 15
Verification and Validation
451
. Here the predicted accelerations at the base and tip of the plate and as well as at
the suspended mass have been plotted versus frequency. The results show the correct response.
Namely, resonant spikes are clearly evident at each of the predicted natural frequencies. The acceleration plot for the end mass shows a single resonance point since only one modes exit below 100 hertz. In contrast, the acceleration plot for the plate tip shows three distinct resonance peaks that correspond to the three predicted modes. A constant unit acceleration is predicted at the base of the plate, indicating that a large enough mass was used when modeling the base in order to impart the desired enforced motion. A comparison of the acceleration profiles plotted
of Problem 24, clearly indicate that nearly
identical results were obtained when using either QUAD4 elements with a standard h-shell formulation or QUAD16 cubic elements with a p-formulation. The actual peak accelerations that were obtained with both element types are summarized below.
Table 15-17 Peak Accelerations for Suspended Mass
Element Type
QUAD4
QUAD16
%, Difference
Peak Acceleration, Mode 1
2.798
2.795
-0.107%
Element Type
QUAD4
QUAD16
%, Difference
Table 15-18 Peak Accelerations for Plate Tip
Mode 1
1.170
1.170
0.0%
Mode 2
3.448
3.480
0.928%
Mode 3
2.084
2.168
4.03%
File(s):
<install_dir>/results_vv_files/prob025.bdf, prob025.op2
14
452
PART 6
Results Postprocessing
14
Figure 15-51 p-Element Model of Plate with Suspended Mass.
Figure 15-52 Acceleration Responses of Plate Tip, End Mass, and Base.
CHAPTER 15
Verification and Validation
453
Problem 26: Complex Modes, Direct Method
Solution/Element Type:
MSC.Nastran, Complex Modes, Solution 107, CBAR, CONM2, CELAS1, and CDAMP Elements.
Reference:
Thompson, W.T., Theory of Vibration With Applications, Prentice-Hall,1972, pp. 23-27.
Blevins, R.D., Formulas For Natural Frequency And Mode Shape, Kreiger Publishing Co., 1979, p. 77.
Problem Description:
Three equal masses are each supported by a massless pendulum. Each pendulum is in turn coupled to the other two pendulums by a linear spring. In addition, there is a rotational damper located at the pivot point for each pendulum. Assuming that each damper has a different strength, determine the complex modes and natural frequencies for this coupled spring-mass system.
Engineering Data:
L = 5 inches a = 5 inches k = 500 lbf / inch
M = 0.01 lbf - sec
2
/ inch
C
1
= 120 lbf - sec
C
2
= 60 lbf - sec
C
3
= 20 lbf - sec
Theoretical Solution:
For the undamped case, there are three modes associated with the angular displacements for each pendulum. The relative angular displacement for each mode are as follows:
θ
1
θ
2
θ
3
=
1
1
1
,
1
0
– 1
,
1
– 2
1
The corresponding natural frequencies associated with each mode are
f
1
=
L
1/2
, f
2
=
L
+
2
-----------
ML
1/2
, f
3
=
L
+
3ka
2
------------
ML
2
1/2 where g refers to gravitational constant, or 386.4 inches/sec
2
. Substituting in the assumed engineering values yields the following undamped natural frequencies:
f
1
= 1.399 hertz , f
2
= 35.616 hertz , f
3
= 61.656 hertz
When damping is present, the damped natural frequency is given by the expression:
14
454
PART 6
Results Postprocessing
14
ω
d
=
ω
n
1
–
ζ
2 where
ω
d
=
ω
n
1 –
ζ
2
ζ
= critial damping ratio
=
c c r i t
and c crit is the critical damping required to just suppress any oscillatory motion. For a simple pendulous mass, c crit can be expressed as:
c c r i t
=
2ML
2
ω
n
To estimate the natural frequencies for the three damped oscillators, the average critical damping ratio is computed.
c
=
120 + 60
3
+ 20
= 66.67 lbf - sec
For the first mode, all of the masses are moving in unison. Thus, the most highly damped pendulum would dominate. However, since this pendulum has a damping rate of 120 lbf - sec, this yields a value of
ζ >
1
, indicating that an overdamped situation should exist so that a non oscillatory mode with essentially zero frequency should result.
Similarly, the second pendulum has a damping rate of 60 lbf - sec which is approximately equal to the average overall damping. Thus,
ζ ≈
1 is equal to one, a critically damped situation exists which is once again characterized by nonoscillatory motion. Thus, there should be a second damped mode characterized by a natural frequency essentially equal to zero.
In the case of the second undamped mode, the motion is confined principally to the first and third pendulums. The lack of motion at the center pendulum effectively isolates the more lightly damped pendulum, thereby permitting an oscillatory motion to occur. Estimating the critical damping on the basis of the second undamped natural frequency gives:
c c r i t
=
(
2ML
2
) × (
2
π
f
2
)
=
111.891 lbf - sec and
ζ ≈
c c r i t
≈
66.667
0.595
111.891
≈
This gives an estimated damped frequency for the second mode that is equal to:
f d m o d e
2
≈
f
2
1
–
ζ
2
≈
28.626 hertz
Similarly, for the third undamped mode, the critical damping is
c c r i t
=
193.698 lbf - sec and
CHAPTER 15
Verification and Validation
455
ζ ≈
c c r i t
≈
66.667
0.344
193.891
≈
This gives an estimated damped frequency of
f d m o d e
3
≈
f
3
1
–
ζ
2
≈
57.896 hertz
MSC.Nastran Results:
To compute the complex modes for the coupled pendulums, the model shown in
was generated using MSC.Patran. The pendulums were modeled with a single massless CBAR element while the end masses were modeled using lumped CONM2 concentrated mass elements. The springs were modeled with CELAS1 linear springs while grounded CDAMP1 elements were used for the rotational dampers.
Using this model, the complex modes were recovered. The following natural frequencies were predicted for each complex mode:
2
3
4
Mode
1
Table 15-19 Predicted Complex Modal Frequencies
Frequency (Hertz)
1.994 x 10
-20
4.776 x 10
-12
27.129
55.802
The corresponding mode shapes were plotted using MSC.Patran and are shown in
. Because of the presence of nonuniform damping, animation of any
one of these modes will show a distinct phase difference in the motion of the individual pendulums.
The complex modal frequencies agree quite closely with the estimated values. As expected, the first two modes involve motion of all three pendulums. The higher damping associated with two of the pendulums produces an overdamped condition which results in a modal frequency of essentially zero. The third mode primarily involves motion of the outermost pendulums, which corresponds to the second undamped mode shape. The predicted value of 27.129 hertz for this mode agrees very closely with the estimated value of 28.626 hertz. Similarly, the fourth mode is characterized primarily by motion at the center pendulum which corresponds to the third undamped mode. The predicted modal frequency of 55.802 hertz once again agrees very favorably with the estimated value of 57.896 hertz.
14
456
PART 6
Results Postprocessing
File(s):
<install_dir>/results_vv_files/prob026.bdf, prob026.op2
14
Basic Model with
Boundary
Conditions
Figure 15-53 Model of Coupled Pendulums.
Mode 1
Freq = 1.9947E-20 Hz
Figure 15-54 Complex Mode 1 of Pendulums, Freq = 1.9994E-20 Hz.
Mode 2
Freq = 4.776E-12 Hz
CHAPTER 15
Verification and Validation
457
14
Figure 15-55 Complex Mode 2 of Pendulums, Freq = 4.776E-12 Hz.
Mode 2
Freq = 27.129 Hz
Figure 15-56 Complex Mode 3 of Pendulums, Freq = 27.129 Hz.
458
PART 6
Results Postprocessing
14
Mode 4
Freq =55.802 Hz
Figure 15-57 Complex Mode 4 of Pendulums, Freq = 55.802 Hz.
CHAPTER 15
Verification and Validation
459
Problem 27: Steady State Heat Transfer, Multiple Cavity Enclosure
Radiation
Solution/Element Type:
MSC.Nastran, Steady State Thermal Analysis, Solution 153, CQUAD4, CHBDYG, and RADCAV
Elements
Reference:
MSC.Nastran Thermal Analysis User’s Guide, Vol. 68, pp. 154-158.
Problem Description:
Four parallel plates radiate to each other and to the external ambient environment, assumed to be a perfect blackbody at a temperature of zero degrees K. If one of the plates is held at a constant temperature of
2000
°
K
, find the temperature of the other three plates.
Engineering Data:
A
= area of plates = 1.0 meters
2
ε
= emmisivity =
α
= absorptivity = 1.0
T
∞
=
0.0
°
K
σ
= 5.67
×
10
– 8
W / m
°
K
4
14
Theoretical Solution:
For the four parallel plates, the theoretical value of the view factor, F, between successive plates is F = 0.2
Thus,
AF
=
5.0
A
(
1
–
F
)
=
0.8
=
1.25
T
1
= 2000.0
°
K
ε
= 1.0
1 –
ε
ε
A
=
0.0
460
PART 6
Results Postprocessing
14
σ
T
4
1.0206
=
σ
T
4
–
5.0
σ
T
4
--------------------------------
+
σ
T
1.25
4
------------
σ
T
4
–
σ
T
4
--------------------------------
5.0
=
σ
T
2
4
–
5.0
σ
T
4
--------------------------------
+
σ
T
4
0.625
σ
T
4
–
σ
T
4
--------------------------------
5.0
=
σ
T
3
4
–
5.0
σ
T
4
--------------------------------
+
σ
T
4
-------------
0.625
σ
T
4
–
5.0
σ
T
4
--------------------------------
=
σ
T
1.25
4
------------
Solving for
T
1
T
2
T
3
and T
4
gives:
T
2
=
1127.57
°
K
T
3
=
637.28
°
K
T
4
= 426.18
°
K
MSC.Nastran Results:
To solve for the temperatures of the plates, the model shown in
using MSC.Patran. The model consisted of 4 CQUAD4 elements. The radiation heat transfer was modeled using three separate radiation cavities that ignored the effects of any shading caused by the intermediate plates. In addition, no ambient element was specified which in effect simulated the effect of having a perfect black body at zero degrees kelvin to model the far field ambient conditions.
The resultant steady state temperatures that were calculated for each of the plates are shown plotted in
. The corresponding radiation heat fluxes are plotted in
along with the actual nodal values for the radiation heat flux. Closer examination of the nodal fluxes reveals the tremendous decrease that occurs in the heat flux when multiple parallel plates are present.
Table 15-20 Steady State Temperatures in Parallel Plates
Source
Theory
MSC.Nastran
%, Difference
T
2
1127.57
1127.46
0.01%
T
3
637.28
637.17
0.02%
T
4
426.18
426.06
0.03%
File(s):
<install_dir>/results_vv_files/prob027.bdf, prob027.op2
Basic Model with Applied Temperature
CHAPTER 15
Verification and Validation
461
14
Figure 15-58 Model of Four Parallel Plates.
Temperature, Deg K
Figure 15-59 Steady State Temperatures of the Four Parallel Plates.
462
PART 6
Results Postprocessing
Radiation Heat Flux,
Watts/Meter
2
14
Figure 15-60 Radiation Heat Fluxes of the Four Parallel Plate.
CHAPTER 15
Verification and Validation
463
Problem 28: Transient Heat Transfer with Phase Change
Solution/Element Type:
MSC.Nastran, Transient Thermal Analysis, Solution 159, CHEX8, CHBDYG, and CONV
Elements.
Reference:
MSC.Nastran Thermal Analysis User’s Guide, Vol. 68, pp. 188-191.
Problem Description:
A cube of water is exposed to an ambient environment that is below the freezing point of water.
In addition, the water is at an uniform initial temperature that is above the freezing point. Forced convection occurs along the lateral faces of the cube. Determine the time it takes for freezing to first occur as well as the total time required for all of the water to freeze.
Engineering Data:
l
= 0.1 meter
h
= convective film coefficient = 100 W/m
2
°
C
L
= latent heat of formation = 3.34
×
10
5
J / kg
T c
= freezing poing = 0
°
C
∆
T
=
2.0
°
C
= temperature range for freezing
T
∞
= ambient temperature =-20.0
°
C
T i n i ti a l
= initial temperature
y l x z
Theoretical Solution:
If no phase change occurs, the heat balance equation is:
ρ
c p
V dt
= –
(
–
T
∞
)
Assuming constant properties, then
ρ
c p
V
[ (
–
T
∞
)
/ T
2
–
T
∞
) ]
=
(
2
–
T
1
)
The elapsed time required for complete freezing to occur is calculated from the following expression:
∆
t c
=
ρ (
+
c p
∆
T
)
/ hA T
c
+
0.5
∆
T
–
T
∞
)
For this specific problem:
A
= 0.06 m
2
,
V
= 0.001 m
3
,
T c
= 0.0
°
C
, ∆
T
= 2.0
°
C
,
14
464
PART 6
Results Postprocessing
14
L
=
3.34
×
10
5
J / Kg, h = 100.0 W/ m
2
, ρ
w
=
1000.0 Kg / m
3
c
=
4217 J /Kg
°
C
,
Substituting these values into the preceding equations gives: time to initiate freezing = t
c
= 420 seconds total phase change time =
∆
t c
= 2718 seconds
MSC.Nastran Results:
To model the freezing of the unit cube of water, the model shown in
using MSC.Patran. The cube was meshed with a single CHEX8 element. A uniform convective boundary condition was imposed along all of the exposed faces of the cube along with an initial temperature of -20 o
C. The properties of water were assigned to the solid element and it was assumed that freezing would initiate at 0 o
C and occur over a temperature range of 2 o
C. A transient analysis was then performed with MSC.Nastran using a fixed time step 5 seconds for a total duration of 5000 seconds.
Using MSC.Patran, the temperature history was plotted for a single node situated at the base of the cube. The results are shown in
. Examining this figure, it is quite evident when
the water began to freeze since the temperature will level off due to the release of the latent heat associated with the formation of ice. Once freezing has completed, the temperature will continue to decline until it reaches the ambient temperature, or
–
20
°
C
.
The corresponding rate of change in enthalpy is shown in plotted in
enthalpy is just the product of the specific heat and temperature, during a phase change the rate of change of enthalpy should remain fairly constant. Afterward, the enthalpy will continue to decline at a decreasing rate as the ice asymptotically approaches the ambient temperature. This
behavior is clearly evident in
Table 15-21 Transient Temperature Results
Source
Theory
MSC.Nastran
%, Difference
t c
,(seconds)
420
430
2.38%
∆
t c
,(seconds)
2718
3100
14.05%
File(s):
<install_dir>/results_vv_files/prob028.bdf, prob028.op2
Basic Model with
Convection Conditions
Figure 15-61 Model of Freezing Cube.
CHAPTER 15
Verification and Validation
465
14
Figure 15-62 Temperature Response of Freezing Cube.
466
PART 6
Results Postprocessing
14
Figure 15-63 Rate of Enthalpy Change of Freezing Cube.
CHAPTER 15
Verification and Validation
467
Problem 29: Steady State Heat Transfer, 1D Conduction and
Convection
Solution/Element Type:
MSC.Nastran, Steady State Thermal Analysis, Solution 153, CROD, CHBDYP, and CONV
Elements.
Reference:
Chapman, A.J., Heat Transfer, 3rd ed., New York, MacMillan Publishing Co., Inc., 1974, p. 76.
Problem Description:
A fin of circular cross section is maintained at 250 ambient temperature of 70 o surface convective film coefficient of 1.6 Btu / hr-ft o
2
F at one end. The fin extends into air at an
F. Assuming a material conductivity of 132 Btu /hr-ft-
o o
F and a
F, determine the steady state temperature distribution along the length of the rod.
Engineering Data:
L = 1 ft d = diameter = 0.04167 ft
A = lateral area = 0.001365 ft
2 k = thermal conductivity = 132 Btu / hr-fto
F h = convective film coefficient = 1.6 Btu / hrft
2
o
F
T base
= 250 o
F
T fluid
= 70 o
F
TBASE = 250 oF
L
TFLUID = 70 oF d
Theoretical Solution:
Assuming only 1D heat transfer along the length of the fin as well as no convective heat loss at the tip, the theoretical temperature distribution is
T
=
(
T ba s e
–
T f l u i d
)
cosh ml cosh
–
ml x
where
m
=
kd
=
4
0.63
×
×
1.6
14
= 1.079
ft
468
PART 6
Results Postprocessing
14
Substituting for m, gives the following steady state temperatures at four positions along the fin.
.25
.50
.75
1.00
X / L T (
o
F)
217.0243
196.0559
183.7156
179.7002
MSC.Nastran Results:
To compute the temperature distribution for the cooling fin, the model shown in
was generated using MSC.Patran. The fin was modeled using 4 CROD elements. By doing so, this enabled the convective boundary condition to be modeled with line type CHBDYP convective boundary elements which alleviated the need to compute the lateral surface area associated with each node. Instead, this was determined by MSC.Nastran from the crosssectional area that was given for the rod.
Using the model shown in
, the nodal temperatures were computed. A fringe plot
of the steady state temperature distribution that was generated by MSC.Patran is shown in
. Here the fringe labels have been included to better show the actual nodal values.
Source
Theory
MSC.Nastran
%, Difference
Table 15-22 Temperatures Along Cooling Fin
X / L
.25
217.0243
217.7879
0.035%
.50
196.0559
196.3183
0.013%
.75
183.7156
184.0306
0.172%
1.00
179.7002
180.0316
0.184%
File(s):
<install_dir>/results_vv_files/prob029.bdf, prob029.op2
Basic Model with Convection Conditions
CHAPTER 15
Verification and Validation
469
14
Figure 15-64 Model of Cooling Fin.
Figure 15-65 Nodal Temperatures of Cooling Fin.
470
PART 6
Results Postprocessing
14
Problem 30: Freebody Loads, Pinned Truss Analysis
Solution/Element Type:
MSC.Nastran, Linear Statics, Solution 101, CROD Elements.
Reference:
Przemieniecki, J.S., Theory of Matrix Structural Analysis, McGraw-Hill, Inc., 1968, p. 155.
Problem Description:
A pinned joint truss is loaded with a force at one end and one of the components is heated uniformly to an elevated temperature. Considering thermal effects, determine the freebody loads for each of the members in the truss.
Engineering Data:
Problem 8: Linear Statics, Pinned Truss Analysis
freebody forces will be plotted.
E
=
1.0
×
10
7
α
= 1.0
×
10
– 6
/ Deg F
A
1
=
1.0 in
2
(Elements 1, 3, 5 and 6)
A
2
=
0.7071068 in
2
(Elements 2 and 4)
∆
T
=
+100. Deg F (Elements 3 only)
F
=
1000.0 lb.
3
2
1
6
F
5 4
T
l
=
20. in
Theoretical Solution:
Problem 8: Linear Statics, Pinned Truss Analysis
MSC.Nastran Results:
Using the model shown in
, the same results were obtained with MSC.Nastran as
Problem 8: Linear Statics, Pinned Truss Analysis
(p. 366). The MSC.Patran Freebody
application was used to determine freebody force associated with every member of the truss.
The resultant freebody forces computed by MSC.Patran are shown in
through
. The freebody forces should be identical to the predicted rod forces which they are.
The freebody forces and moments for the entire truss are plotted in
. The freebody moments are labeled in blue and are all zero in order to maintain rotational equilibrium. The
File(s):
<install_dir>/results_vv_files/prob030.bdf, prob030.op2
Basic Model with Loads and BCs
Figure 15-66 Model of Pinned Truss.
CHAPTER 15
Verification and Validation
471
14
Freebody Force
Bar 1
Figure 15-67 Freebody Forces in Bar 1.
472
PART 6
Results Postprocessing
14
Freebody Force
Bar 2
Figure 15-68 Freebody Forces in Bar 2.
Freebody Force
Bar 3
Figure 15-69 Freebody Forces in Bar 3.
Freebody Force
Bar 4
Figure 15-70 Freebody Forces in Bar 4.
Freebody Force
Bar 5
CHAPTER 15
Verification and Validation
473
14
Figure 15-71 Freebody Forces in Bar 5.
474
PART 6
Results Postprocessing
14
Freebody Force
Bar 6
Figure 15-72 Freebody Forces in Bar 6.
Frebody Forces and Moments
Entire Truss
Figure 15-73 Freebody Forces and Moments for Entire Truss.
487
I N D E X
MSC.Patran Reference Manual
Part 6: Results Postprocessing
I N D E X
MSC.Patran
Reference
Manual
Part 6: Results
Postprocessing
A
animation options, 44, 47, 168, 170
attributes
B
C
complex results
coordinate systems, 42 global projected, 42
D
plot attributes, 8 plot targets, 8
Index
488
INDEX
Index
display attributes
tensors, 107, 136 vectors, 107, 136 display attributes, scalars, 136
G
H
E
animation, 51, 64, 83, 116, 173
combined plot, 50, 51, 65, 84, 98, 99, 117,
F
I
insight forms, 256 insight imaging, 256
isosurface attributes, 267 form, 267
isosurface coordinate selection, 265
L
M
maximum shear stress, 298, 303
N
INDEX
489
O
octahedral shear stress, 298, 300
P
plot options
markers, 111, 137 tensors, 111, 137 vectors, 111, 137 plot options, scalars, 137
plots
animation, 6 deformation, 6 freebody, 6 fringe, 6
Q
R
report
result cases, 5, 293 result data types, 293
results
S
sorting
T
tensors, 105, 135 vectors, 105, 135 target entities, scalars, 135
tensor
Index
490
INDEX
U
using templates for results plots, 23
V
X
Index
Télécharger
Lien public mis à jour
Le lien public vers votre chat a été mis à jour. Vous pouvez afficher et gérer vos liens de chat après inscription ici.
Lien public du document
Publicité
