HowTo How To

: Ensight Howto HowTo EnSight92_Docs

Open the PDF directly: View PDF .
Page Count: 443

Download
Open PDF In Browser	View PDF

Index

Alphabetical Listing

Table of Contents

Introduction
Use the Online Documentation
Using The How To Manual
EnSight Overview
Connect EnSight Client and Server
Command Line Start-up Options
Use Environment Variables
Use MPI

Read and Load Data
Read Data
Use ens_checker
Load Multiple Datasets (Cases)
Load Transient Data
Use Server of Servers
Load Spatially Decomposed Case Files
Read User Defined
Do Structured Extraction
Use Block Continuation
Use Resource Management

Save or Output
Save or Restore an Archive
Record and Play Command Files
Print/Save an Image
Save Geometric Entities
Save/Restore Context
Save Scenario
Save/Restore Session
Output for Povray

Manipulate Viewing Parameters
Rotate, Zoom, Translate, Scale
Set Drawing Mode (Line, Surface, Hidden Line)
Set Global Viewing Parameters
Set Z Clipping
Set LookFrom / LookAt
Set Auxiliary Clipping
Define and Change Viewports
Control Lighting Attributes
Display Remotely
Save and Restore Viewing Parameters
Create and Manipulate Frames
Reset Tools and Viewports
Use the Color Selector
Enable Stereo Viewing
Pick Center of Transformation
Set Model Axis/Extent Bounds
Do Viewport Tracking
View a Viewport Through a Camera
Manage Views

Manipulate Tools
Use the Cursor (Point) Tool
Use the Line Tool

Use the Plane Tool
Use the Box Tool
Use the Cylinder Tool
Use the Sphere Tool
Use the Cone Tool
Use the Surface of Revolution Tool
Use the Selection Tool
Use the Spline Tool

Visualize Data
Introduction to Part Creation
Create Contours
Create Isosurfaces
Create Particle Traces
Create Clips
Create Clip Lines
Create Clip Planes
Create Box Clips
Create Quadric Clips
Create IJK Clips
Create XYZ Clips
Create RTZ Clips
Create Revolution Tool Clips
Create Revolution of 1D Part Clips
Create General Quadric Clips
Create Clip Splines
Create Vector Arrows
Create Elevated Surfaces
Extrude Parts
Create Profile Plots
Create Developed (Unrolled) Surfaces
Create Subset Parts
Create Tensor Glyphs
Display Displacements
Display Discrete or Experimental Data
Change Time Steps
Extract Vortex Cores
Extract Separation and Attachment Lines
Extract Shock Surfaces
Create Material Parts
Remove Failed Elements
Do Element Blanking
Use Point Parts

Create and Manipulate Variables
Activate Variables
Create New Variables
Extract Boundary Layer Variables
Edit Color Palettes
Use Volume Rendering

Query, Probe, Plot
Get Point, Node, Element, and Part Information
Probe Interactively
Query/Plot
Page 1

Change Plot Attributes
Query Datasets

Manipulate Parts
Change Color
Copy a Part
Group Parts
Merge Parts
Extract Part Representations
Cut Parts
Delete a Part
Change the Visual Representation
Set Attributes
Display Labels
Set Transparency
Select Parts
Set Symmetry
Map Textures

Animate
Animate Transient Data
Create a Flipbook Animation
Create a Keyframe Animation
Animate Particle Traces

Annotate
Create Text Annotation
Create Lines
Create 2D Shapes
Create 3D Arrows
Create Dials
Create Gauges
Load Custom Logos
Create Color Legends
Manipulate Fonts

Configure EnSight
Customize Icon Bars
Customize Mouse Button Actions
Save GUI Settings
Define and Use Macros
Set or Modify Preferences
Enable User Defined Input Devices
Produce Customized Pop-Up Menus
Produce Customized Access to Tools & Features
Setup For Parallel Computation
Setup For Parallel Rendering

Miscellaneous
Select Files

Page 2

Print/Save an Image, 98
Activate Variables, 273
Animate Particle Traces, 365
Animate Transient Data, 348
Change Color, 314
Change Plot Attributes, 305
Change the Visual Representation, 322
Change Time Steps, 256
Command Line Start-up Options, 22
Connect EnSight Client and Server, 12
Control Lighting Attributes, 142
Copy a Part, 316
Create 2D Shapes, 373
Create 3D Arrows, 375
Create a Flipbook Animation, 351
Create a Keyframe Animation, 355
Create and Manipulate Frames, 145
Create Box Clips, 222
Create Clip Lines, 214
Create Clip Planes, 217
Create Clip Splines, 236
Create Clips, 213
Create Color Legends, 383
Create Contours, 198
Create Developed (Unrolled) Surfaces, 247
Create Dials, 377
Create Elevated Surfaces, 243
Create Gauges, 380
Create General Quadric Clips, 234
Create IJK Clips, 225
Create Isosurfaces, 200
Create Lines, 371
Create Material Parts, 265
Create New Variables, 275
Create Particle Traces, 204
Create Profile Plots, 246
Create Quadric Clips, 223
Create Revolution of 1D Part Clips, 233
Create Revolution Tool Clips, 232
Create RTZ Clips, 230
Create Subset Parts, 248
Create Tensor Glyphs, 249
Create Text Annotation, 367
Create Vector Arrows, 238
Create XYZ Clips, 228
Customize Icon Bars, 390
Customize Mouse Button Actions, 392
Cut Parts, 320
Define and Change Viewports, 133
Define and Use Macros, 395
Delete a Part, 321
Display Discrete or Experimental Data, 254
Display Displacements, 251
Display Labels, 329
Display Remotely, 143
Do Element Blanking, 269
Do Structured Extraction, 73
Do Viewport Tracking, 159
Edit Color Palettes, 285

Enable Stereo Viewing, 155
Enable User Defined Input Devices, 416
EnSight Overview, 10
Extract Boundary Layer Variables, 283
Extract Part Representations, 319
Extract Separation and Attachment Lines, 261
Extract Shock Surfaces, 263
Extract Vortex Cores, 259
Extrude Parts, 244
Get Point, Node, Element, and Part Information, 291
Group Parts, 317
Introduction to Part Creation, 191
Load Custom Logos, 382
Load Multiple Datasets (Cases), 52
Load Spatially Decomposed Case Files, 66
Load Transient Data, 57
Manage Views, 162
Manipulate Fonts, 386
Map Textures, 338
Merge Parts, 318
Output for Povray, 116
Pick Center of Transformation, 156
Probe Interactively, 294
Produce Customized Access to Tools & Features, 424
Produce Customized Pop-Up Menus, 417
Query Datasets, 313
Query/Plot, 297
Read Data, 36
Read User Defined, 72
Record and Play Command Files, 95
Remove Failed Elements, 267
Reset Tools and Viewports, 152
Rotate, Zoom, Translate, Scale, 120
Save and Restore Viewing Parameters, 144
Save Geometric Entities, 106
Save GUI Settings, 394
Save or Restore an Archive, 92
Save Scenario, 112
Save/Restore Context, 110
Save/Restore Session, 115
Select Files, 434
Select Parts, 332
Set Attributes, 324
Set Auxiliary Clipping, 132
Set Drawing Mode (Line, Surface, Hidden Line), 123
Set Global Viewing Parameters, 125
Set LookFrom / LookAt, 129
Set Model Axis/Extent Bounds, 157
Set or Modify Preferences, 399
Set Symmetry, 335
Set Transparency, 331
Set Z Clipping, 127
Setup For Parallel Computation, 432
Setup For Parallel Rendering, 433
Use Block Continuation, 79
Use ens_checker, 46
Use Environment Variables, 28
Use MPI, 31
Use Point Parts, 271

Page 3

Use Resource Management, 84
Use Server of Servers, 59
Use the Box Tool, 174
Use the Color Selector, 154
Use the Cone Tool, 181
Use the Cursor (Point) Tool, 164
Use the Cylinder Tool, 177
Use the Line Tool, 166
Use the Online Documentation, 5

Use the Plane Tool, 169
Use the Selection Tool, 186
Use the Sphere Tool, 179
Use the Spline Tool, 189
Use the Surface of Revolution Tool, 183
Use Volume Rendering, 289
Using The How To Manual, 7
View a Viewport Through a Camera, 160

Page 4

Introduction
Use the Online Documentation

INTRODUCTION
The EnSight online documentation consists of:
Installation Guide

Consists of a .pdf file in the doc directory (as well as being available for easy reading
from the web install page). Also goes out as hardcopy with an EnSight distribution CD.

Getting Started
Manual

The Getting Started Manual contains basic Graphical User Interface overview
information and several tutorials. This manual is not cross-referenced with any of the
other manuals.

How To Manual

The How To documentation consists of relatively short articles that describe how to
perform a specific operation in EnSight, such as change the color of an object or
create an isosurface. Step-by-step instructions and pictures of relevant dialogs are
included. In addition, each How To article typically contains numerous hyperlinks
(colored blue) to other related articles (and relevant sections of the User Manual).
Note that, although the entries in the How To table of contents and index are not
colored blue, you can still click on an entry and jump to the appropriate document.
How To Use the How To Manual
How To Table of Contents
How To Index

User Manual

The User Manual is a more traditional document providing a detailed reference for
EnSight. The User Manual contains blue hyperlinks as well. Both the User Manual
table of contents and index entries are hotlinked as well as cross-reference entries
within chapters (which typically start with “See Section ...” or “See How To ...”).
User Manual Table of Contents
User Manual Index

Command Language
Manual

The Command Language Reference Manual documents command language used
within EnSight. This manual contains some cross-references to the How To and User
Manuals, but cross-referencing from them back is extremely minimal.

Interface Manual

The Interface Manual contains the information needed for creating user-defined
readers, creating user-defined writers, creating user-defined math functions,
interacting with EnSight through the external command driver, and using the EnSight
python interpreter.

WHERE TO START?
If you are new to EnSight you should read the EnSight Overview article. Chapter 1 and Chapter 5 in the User
Manual also provide overview information. The Introduction to Part Creation provides fundamental information on
EnSight’s part concept.

PDF READER
The EnSight online documentation is in pdf format. EnSight uses a pdf reader such as the Acrobat® Reader software
from Adobe Systems, Inc., Xpdf, or Apple’s Preview. Any of these readers provide similar capabilities. For the
purposes of this documentation, the Acrobat Reader will be pictured. A pdf reader provides much the same
functionality as a World Wide Web browser while providing greater control over document content quality. To use a
different reader (from the default), simply set the environment variable CEI_PDFREADER to a different reader
application. See How To Use the How To Manual for more information on using a pdf reader.

Page 5

HOW TO PRINT THE DOCUMENTATION
Printing Topics From a PDF Reader
You can easily print any topic in the How To manual or any pages from the other documentation from within the pdf
reader. The documents have been optimized for screen manipulation, but will still produce decent hardcopy printouts.
To print a topic:
1. Navigate to the topic you want to print.
2. Choose Print... from the File menu.
3. Be sure the Printer Command setting is correct for your environment and then click OK. Your document should
print to the selected (or default) printer. If you do not have a printer available on your network or you wish to save
the PostScript file to disk, you can do so: click the File button, enter a filename, and click OK.

Printing EnSight Manuals
You can print (all or portions of) the EnSight manuals from provided .pdf files. These files have been print optimized
and should produce reasonably high quality hardcopy. They have all been formatted for letter size paper. These files
are located in the doc/Manuals directory of the EnSight installation.
$CEI_HOME/ensight92/doc/Manuals/GettingStarted.pdf
$CEI_HOME/ensight92/doc/Manuals/HowTo.pdf
$CEI_HOME/ensight92/doc/Manuals/UserManual.pdf
$CEI_HOME/ensight92/doc/Manuals/CLmanual.pdf
$CEI_HOME/ensight92/doc/Manuals/InterfaceManual.pdf
You can open these manuals in the pdf reader and print any or all pages, or send them to an outside source for
printing, or order printed copies from our website.

CONTACTING CEI
If you have questions or problems, please contact CEI:
Computational Engineering International, Inc.
2166 N. Salem Street, Suite 101
Apex, NC 27523 USA
Email:
Hotline:

support@ensight.com
800-551-4448 (U.S.)
919-363-0883 (Non-U.S.)

Phone:
FAX:

919-363-0883
919-363-0833

WWW:

http://www.ceintl.com

or

http://www.ensight.com

Page 6

Using The How To Manual

INTRODUCTION
The “How To” documentation provides quick access to various topics of interest. The topics provide basic and some
advanced usage information about a specific tool or feature of EnSight. Each topic will provide links to the
appropriate section of the EnSight User Manual as well as links to other applicable How To articles. When you hit a
Help button within the various dialogs in EnSight, you will generally be taken to one of the topics in the “How To”
manual.
Topics typically contain the following sections:
Introduction

Introduction to the topic

Basic Operation

Quick steps for simple usage

Advanced Usage

Detailed information on topic

Other Notes

Other items of interest

See Also

Links to related topics and documentation

(See below for how to quickly jump to a specific section using document navigation.)
The header and footer of each article page provides simple navigation controls:
Return to How To
Topics List

Access this page

First page of
current topic

Previous page

Last page of
current topic

Next page

In addition, links to other documents are displayed as highlighted text. Note that all links and navigation controls
(except index and table of contents) are colored blue.

PDF READER
The EnSight online documentation is in .pdf format. EnSight uses a pdf reader such as the Acrobat® Reader software
from Adobe Systems, Inc., Xpdf, or Apple’s Preview. Any of these readers provide similar capabilities. For the
purposes of this documentation, the Acrobat Reader is pictured. A pdf reader provides much the same functionality
as a World Wide Web browser while providing greater control over document content quality. To use a different pdf
reader, simply set the environment variable CEI_PDFREADER to a different reader application.
The user interface for the various pdf readers is very simple and provides intuitive navigation controls. Keep in mind
that the pages were designed to be viewed at 100% magnification. Although you can use other magnification
settings, the quality of the dialog images may be degraded.

Page 7

Thus, in addition to the navigation controls within the document itself which are described above, a pdf reader
(Acrobat for example) provides quick access to various display options and navigation controls. A few of them are
pointed out for the Acrobat Reader below. Please use the Help option for your reader for a more comprehensive
description of its options.
Select Tool
Grab and move page
Print

Click and zoom in
(Ctl-click to zoom out)
Standard page
magnification controls
For additional help

Standard page
navigation

Go forward to previously
viewed page
Go back to last
viewed page

Each How To topic provides a set of bookmarks that match the standard
section titles. You can quickly navigate to one of these sections by using
the bookmark list in pdf reader.
The “Go back/forward” buttons are particularly useful – they operate somewhat like the “Back” and “Forward” buttons
on standard Web browsers. If your previously viewed page was in a different document, the pdf reader will
automatically reload the appropriate file and jump to the correct page. Note that most pdf readers also consider a
change of view (e.g. scrolling) or magnification as an event to remember in the back/forward list.

Page 8

PRINTING
Printing Topics From The PDF Reader
You can easily print any topic in the How To manual or pages from the other documentation from within the pdf
reader. The documents will produce decent hardcopy printouts. To print a topic:
1. Navigate to the topic you want to print.
2. Choose Print... from the File menu (or hit the printer icon).
3. Be sure the Printer Command setting is correct for your environment and then click OK. Your document should
print to the selected (or default) printer. If you do not have a printer available on your network or you wish to save
the PostScript file to disk, you can do so: click the File button, enter a filename, and click OK.

Printing EnSight Manuals
You can print (all or portions of) the EnSight manuals from provided .pdf files. These files have been print optimized
and should produce reasonably high quality hardcopy. They have all been formatted for letter size paper. These files
are located in the doc/Manuals directory of the EnSight installation.
$CEI_HOME/ensight92/doc/Manuals/Installation.pdf
$CEI_HOME/ensight92/doc/Manuals/GettingStarted.pdf
$CEI_HOME/ensight92/doc/Manuals/HowTo.pdf
$CEI_HOME/ensight92/doc/Manuals/UserManual.pdf
$CEI_HOME/ensight92/doc/Manuals/CLmanual.pdf
$CEI_HOME/ensight92/doc/Manuals/InterfaceManual.pdf
You can open these manuals in the pdf reader and print any or all pages, or send them to an outside source for
printing.

Page 9

EnSight Overview

ENSIGHT OVERVIEW
EnSight is a powerful software package for the postprocessing, visualization, and animation of complex datasets.
Although EnSight is designed primarily for use with the results of computational analyses, it can also be used for
other types of data. Please note that EnSight CFD is a separate product.
This document provides a very brief overview of EnSight. Consult Chapter 1 in the User Manual for additional
overview information. This article is divided into the following sections:
Graphical User Interface
Client / Server Architecture
EnSight’s Parts Concept
Online Documentation

Graphical User Interface
The graphical user interface (GUI) of EnSight contains the following major components:
Note: This whole upper level of the GUI
is referred to as the “Desktop”

Information Area Button
Click to see information dialog.
Message Area
Quick Interaction Area
Interface controls associated with the current
feature selected from the Feature Icon Bar.

Main Menu
Feature Icon Bar
Sets the current feature. Click an
icon to open the associated Quick
Interaction area.
Main Parts List
All parts from your model as well as
created parts (e.g. clips, isosurfaces)
are listed here. Click an item to
select part(s) to operate on.
Mode Selection Area
Sets the major mode of EnSight (Part,
Annot, Plot, VPort, ...) and loads the
applicable set of icons into the
vertical Mode Icon Bar. Click the
button to select the Mode.

Mode Icon Bar
The set of icons associated with the
current Mode. Click the icon to
access the function. If Tool Tips are
on (bottom right of desktop), the
icon’s function name will be shown
when mouse is over the icon. If
necessary, use the vertical scroll bar
to access the remainder of the icons.
Transformation Control Area
Buttons that control the current
transformation operation (e.g. rotate
or translate) associated with mouse
action in the Graphics Window. Other
buttons open dialogs providing
detailed transformation control.

Graphics Window showing inset plot and viewport

Chapter 5 in the User Manual provides additional overview information on the user interface.
Page 10

Client / Server Architecture
To facilitate the handling of large datasets and efficiently use networked resources, EnSight was designed to
distribute the postprocessing workload. Data I/O and all compute intensive functions are performed by a server
process. The server transmits 3D geometry (and other information) to a client running on a graphics workstation.
The client handles all user interface interaction and graphic rendering using the workstation’s built-in graphics
hardware.
host1

host2

Server
Requests

Server
3D objects

host1

Client

Client

Stand-alone Operation

Distributed Operation

The client and server each run as separate processes on one or more computers. When distributed between a
compute server and a graphics workstation, EnSight leverages the strengths of both machines. When both tasks
reside on the same machine, a stand-alone capability is achieved. The client–server architecture allows EnSight to
be used effectively, even on systems widely separated geographically.
Before EnSight can be used, the client and server must be connected. For standalone operation, you simply run the
“ensight8” script and the client and server are started and connected for you. For distributed operation (as well as for
standalone operation when more control is desired), there are two methods of achieving a connection: a manual
connection (described in the Getting Started manual) or an automatic connection (described in How To Connect
EnSight Client and Server).
EnSight’s cases feature allows you to postprocess multiple datasets simultaneously. Cases is implemented by
having a single client connected to multiple servers running on the same or different machines.

EnSight’s Parts Concept
One of the central concepts of EnSight is that of the part. A part is a named collection of elements (or cells) and
associated nodes. The nodes and/or elements may have zero or more variables (such as pressure or stress). All
components of a part share the same set of attributes (such as color or line width).
Parts are either built during the loading process (based on your computational mesh and associated surfaces) or
created during an EnSight session. Parts created during loading are called model parts.
All other parts are created during an EnSight session and are called created or derived parts. Created parts are built
using one or more other parts as the parent parts. The created parts are said to depend on the parent parts. If one or
more of the parent parts change, all parts depending on those parent parts are automatically recalculated and
redisplayed to reflect the change. As an example, consider the following case. A clipping plane is created through
some 3D computational domain and a contour is created on the clipping plane. The contour’s parent is the clipping
plane, and the clipping plane’s parent is the 3D domain. If the 3D domain is changed (e.g. the time step changes),
the clipping plane will first be recalculated, followed by the contour. In this way, part coherence is maintained.
One of the major modes of EnSight is Part Mode. Operations in Part Mode (performed by clicking one of the icons in
the vertical Mode Icon bar) operate on the parts currently selected in the Main Parts list. See How To Select Parts
for more information.
See the Introduction to Part Creation for more information on parts.

Online Documentation
Documentation for EnSight is available online. See How To Use the Online Documentation for more information as
well as hyperlinks to the main documents. Online documentation is accessed from the Main Help menu in the user
interface. In addition, major dialog windows contain Help buttons that will open a relevant “How To” article.

Page 11

Connect EnSight Client and Server

INTRODUCTION
EnSight is a distributed application with a client that manages the user interface and graphics, and a server that reads
data and performs compute-intensive calculations. The client and server each run as separate processes on one or
more computers. Before EnSight can do anything useful, the client process must be connected to the server process.
For a simple operation on the same machine (standalone), the client and server processes will be started and
connected for you. If you desire more control over the standalone operation or want to take advantage of a
distributed operation, you have the options described below.

Necessary Prerequisites
EnSight must have been installed, the CEI_HOME and the command search path set properly. If you successfully
performed the installation as described in the Installation Guide, then these settings should be correct.
(See $CEI_HOME/ensight92/doc/Manuals/Installation.pdf if you need this manual.)

SIMPLE STANDALONE OPERATION (CONNECTION OCCURS AUTOMATICALLY)
If you want to run Ensight client and server (or SOS) on the same machine (standalone), and you have not changed
the default automatic connections to be elsewhere, you can simply do the following:
To Start Ensight:
Non Windows:

Windows:

EnSight92

Either double click the EnSight 9.2
icon on the desktop,

or
Start > CEI > EnSight 9.2

At the prompt In a shell window, type:
ensight92

To Start Ensight in SOS mode: (reminder that you need a gold license key for this)
Non Windows:

Windows:
Start > CEI > EnSight 9.2 SOS

At the prompt in a shell window, type:
ensight92 -sos

Note: To add another dataset or replace the existing dataset (which EnSight refers to as another case), see Adding Another Case
below

Page 12

CONNECTING AUTOMATICALLY
Automatic connections are made according to the “default” connection settings that have been stored (and are
visible) in the Job Launch Settings Dialog. The connection that occurs on startup will be according to the settings
saved in this dialog (and its associated file). Thus, it is important that you know how to get to this dialog.
The Job Launch Settings dialog is accessed via Case on the
main menu.
For each connection, fields are provided for
the needed information.
The default connection is indicated with a True
value for ‘Default configuration’. If EnSight is
started with a connection to an existing
Configuration then it uses those settings. For
example,
ensight92 -c remote_conn
will start up with the indicated options. If the
Configuration is not found, then EnSight will
start up with your default settings but then use
the host name as given by the ‘-c’ command
line option.
When you make changes to any of the fields,
the Save button is activated so you can save
these settings.

To add a new entry, click “New”, name your
entry in Configuration name, fill in your data,
toggle the Default configuration toggle if you
wish this to be your default connection setting,
and press “Save” to save your entry.
Working directory is used when the server is
first started and the browser is opened (e.g. for
case add or case replace). If the working
directory is not set, EnSight uses the
preferences directory. If that is not set, then
the current working directory will be
dependent on the platform, operating system,
and user settings.

If a numerical field has a -1 in it or if a string field is empty,
then it uses the default setting for that field. Currently, the
field Number of Nodes should be left to 1.

Page 13

CONNECTING MANUALLY
ensight92.client -cm will start a client that expects a manual connection and will prompt the user to start the
server/SOS manually, you can do something like the following:
Note: the machine you are running the client on will be referred to as CLIENT_HOST.
the machine you desire to run the server on will be referred to as SERVER_HOST
In a second window, log onto the SERVER_HOST machine using telnet (or ssh or equivalent).
The SERVER_HOST does not have to be of the same operating system as the CLIENT_HOST.

Example of doing a telnet from a
linux machine to a unix machine.

Example of doing a telnet
from a windows machine to
a windows machine.

Start the ensight server on the SERVER_HOST machine, using the appropriate script and the -c option.
If the SERVER_HOST machine is
Windows:
ensight92_server -c CLIENT_HOST
Note the difference ( . vs _ )
Non-Windows: ensight92.server -c CLIENT_HOST
or for SOS
Windows:
Non-Windows:

ensight92_sos -c CLIENT_HOST
ensight92.sos -c CLIENT_HOST

Note the difference ( . vs _ )

The -c CLIENT_HOST option tells the EnSight Server to connect to the EnSight Client listening on CLIENT_HOST.

Example if doing a
telnet into a
SERVER_HOST which is a
windows machine

Example if doing a telnet into a
SERVER_HOST which is a linux machine.

The Server should now make the connection. To see if the connection is successful, you can click on the Information

Page 14

button on the Desktop. You should see “Connection accepted” in the EnSight Message Window which comes up. You
can also check the Connection Details under the Case menu. Licensing information should also appear in the
Graphics Window. If the connection failed, please consult Manual Connection Troubleshooting below and
Troubleshooting the Connection in the Installation Guide before contacting CEI support.

Manual Connection Troubleshooting
A manual connection can fail for any of several reasons. Because of the complexity of networking and customized
computing environments, we recommend that you consult your local system administrator and/or CEI support if the
following remedies fail to resolve the problem.
Problem

Probable Causes

Solutions

Unable to telnet into the
SERVER_HOST machine

Telnet service not allowed or not
running on the SERVER_HOST
machine.

Get system administration help to be able to perform this
operation. It may be that your site requires the use of ssh
or some other equivalent.

Ensight server does not start on
SERVER_HOST machine.

EnSight is not properly installed on
the SERVER_HOST

Verify the installation on the SERVER_HOST as described
in the Installation Guide. Making sure that the proper
environment variables and command path have been set.

For Unix Systems:

ADVANCED USAGE
Command Line Options
Command line options can be used to streamline many of the connection processes.Connection Details
Startup Command

Description

ensight92
ensight92.client -c

Starts up client and autoconnects according to default job launch configuration settings.

ensight92 -sos
ensight92.client -c -sos

Starts up client and auto connects to sos according to default job launch configuration
settings. This requires a gold key.

ensight92.client

Starts up client with no connection.

ensight92.client -c connname

Starts up client and auto connects to the host specified in the job launch configuration
settings. The default settings are used if connname is not listed.

ensight92.client -c connname -sos Starts up client and auto connects the sos to the host specified in the job launch configuration
setttings.
ensight92.client -cm

Starts up a client, and prompts for a manual connection.

* Note that if you are starting from a PC in a command window, change the period to an underscore: ensight92.client becomes
ensight92_client. Also if you specify a resource file to use in the start up, it takes precedence over connection settings.

Connection Details
You can always check the status of the current connection by accessing the Connection details dialog from the Case

Page 15

menu.

The Connection details dialog is informational; the fields
cannot be changed by the user.
Press Update to refresh the information, if this dialog has been
open while activity is occurring.

Page 16

Adding Another Case
You would add another case when you want to add an additional dataset (called a “case”) to your EnSight session.
This is often used for things like A-B comparisons or for assembling components that have been analyzed in different
solvers. You can also use the process described below to replace the current case with a new one without having to
restart EnSight.
You can add or replace cases directly from the
Case menu,

From either option, this dialog will
appear when adding a case.

Additionally, this dialog will appear first
when replacing a case.

For more information on Cases, see How To Load Multiple Datasets (Cases)

Page 17

Other Auto connection requirements
The auto-connect mechanism requires that certain conditions exist in your computing environment for auto
connections to work when running the EnSight server or SOS process on a different computer. Specifically, EnSight
depends on a correctly working 'ssh' command that doesn't require passwords. The notes below assume using the
default 'ssh' command.
Alternatively, EnSight can use a replacement command for 'ssh' as long as that replacement command follows 'ssh'
syntax or ‘rsh’ syntax
(i.e. rsh [-l username] hostname command)
Should you wish to use an alternative command for 'ssh', you may specify this command in the Job Launch
Configuration Setting dialog or on the EnSight command line with the '-rsh alternative_command_name' command
line option where 'alternative_command_name' is the replacement command. Typically, one of these mechanisms is
used in computing environments that use either 'ssh' or 'k5rsh'.

On Unix Systems:
1. You have a .cshrc file (even if you are running some other command shell such as /bin/sh) in your home
directory on the EnSight server host that contains valid settings for CEI_HOME, and that your path variable
includes the bin directory of CEI_HOME. For example, if your EnSight distribution is installed in /usr/local/
CEI and you are running EnSight on an Linux or Unix system (other architectures use a different library path
variable), your .cshrc should contain:
setenv CEI_HOME /usr/local/CEI
set path = ( $path $CEI_HOME/bin )
To verify the settings, simply try to start the server.
2. Your .cshrc file (or files sourced or executed from there) has no commands that cause output to be written (e.g.
date or pwd). Any output can interfere with EnSight server startup.
3. You can successfully execute a remote shell command from the client host system to the server host system. The
name of the remote shell command varies from system to system. While logged on to the client host system,
execute one of the following (where serverhost is the name of your server host system):
ssh serverhost date
If successful, the command should print the current date.
If any of these conditions are not met, you will be unable to establish a connection automatically and will have to use
the manual connection mechanism. Note that it is not uncommon for system administrators to disable operation of all
remote commands for security reasons. Consult your local system administrator for help or more information.
Note that if you wish to use ‘rsh’ instead of ‘ssh’, then you need to have a valid .rhosts file in your home directory
on all systems on which you wish to run the EnSight server. The file permission for this file must be such that only the
owner (you) has write permission (e.g. chmod 600 ~/.rhosts). A .rhosts file grants permission for certain
commands (e.g. rsh or rlogin) originating on a remote host to execute on the system containing the .rhosts file.
For example, the following line grants permission for remote commands from host clienthost executed by user
username to execute on the system containing the .rhosts file:
clienthost username
There should be one line like this for every client host system that you wish to be able issue remote commands from.
It is sometimes necessary to add an additional line for each client host of the form clienthost.domain.com
username (where domain.com should be changed to the full Internet domain name of the client host system). To
verify this, simply try to rsh to the remote machine.

On Windows Systems:
1. You have the EnSight server (ensight92_server) installed on the same system as your EnSight client (if you plan to
connect to the same system)
---- OR ---2. You can successfully execute a remote shell command from the client host system to the server host system.

Page 18

Note: By default EnSight will use the ‘ssh’ command. ssh is not a default component on Windows
workstations and must be installed by the user from one of many third party sources. However, Windows
does include a rsh command which EnSight can optionally use. Note, however, only systems running
Windows Server have the RSH service and can respond by executing the EnSight server.
The name of the remote shell command varies from system to system. While logged on to the client host system,
execute one of the following (where serverhost is the name of your server host system):
ssh serverhost date
rsh serverhost date
If successful, the command should print the current date.
If condition 1. or 2. is not met, you will be unable to establish a connection automatically and will have to use the
manual connection mechanism. Note that it is not uncommon for system administrators to disable operation of all
remote commands for security reasons. Consult your local system administrator for help or more information.

Manual connection Troubleshooting
An automatic connection can fail for any of several reasons. Because of the complexity of networking and customized
computing environments, we recommend that you consult your local system administrator and/or CEI support if the
following remedies fail to resolve the problem.
Problem

Probable Causes

Solutions

Server (remote) host name is
incorrect for some reason.

Is the server host entered correctly in the Hostname
field? Try running telnet serverhost from the client
machine.

Incorrect or missing .rhosts file
in your home directory on the
server host.

Follow the instructions on .rhosts files (as described in
the Basic Operation section, step 1 above). If you cannot
successfully execute a remote command (such rlogin
or rsh) from the client host to the server host, you will not
be able to connect automatically.

The user account (i.e. login name)
on the client host does not exist on
the server host.

Enter your login name on the server host in the Login
name field.

The server executable is not found
on the server system

Is the entry in the Executable [path/]name field correct? If
the server executable is NOT in your default command
search path on the server, you must include the full path
name to the executable. For example, /usr/local/
CEI/ensight92/bin/ensight92.server.

Your .cshrc does not contain a
valid setting for CEI_HOME.

Add the appropriate line as described in the Basic
Operation section, step 2 above.

Your .cshrc file (or files executed
by it) causes output to be written.
This is interpreted as a server
startup error.

Remove the offending commands from your .cshrc file.
As a test, do the following:

For Unix Systems:
Automatic connection fails or is
refused

% cd
% mv .cshrc .cshrc-SAVE
Create a new .cshrc file that contains only the lines to set
CEI_HOME and path as described in the Basic
Operation section, step 2 above. If that test works, you
will need to examine your .cshrc to find and remove the
offending lines.

For Windows Systems:
Automatic connection fails or is
refused (trying to connect to
same host system)

Server not installed or not
executable.

You should be able to locate the server executable
(ensight92_server) using Windows Explorer. Double click
on it and see if a console window opens with “This is
EnSight Server 9.2” etc. If this doesn’t happen, refer to
“Troubleshooting the Installation” in the Getting Started
Manual.

Page 19

Problem

Probable Causes

Solutions

Path to the server is incorrect

If using the EnSight Connect dialog, check that the
correct path is specified in the “Executable” field.
If running from the ensight92 command, first ensure that
your PATH environment variable contains the paths for
the ensight92 “client” and “server” directories. You can
check and correct the value of PATH in the Start
>Settings >ControlPanel >System_Environment dialog.

Incorrect hostname entered in the
“Hostname” field of the Connection
settings dialog.

Make sure that the hostname is correct, including the
case of all letters. The ONLY way to confidently see the
hostname (in the correct case) from Windows is to open
a Command Prompt window and type:
> ipconfig /all
The Host Name will be one of the first things listed.

Automatic connection fails or is
refused (trying to connect to a
remote server)

Same causes as for a Unix system

See “For Unix Systems” portion of this table above.

Other Notes
Connection Name - Hostname flexibility
When you specify '-c name' on the command line, EnSight will match the specified 'name' to a Job Launch
Configuration name. If a match is found, then the Configuration’s Hostname (not Configuration name) is used as the
computer name for the EnSight Server or EnSight SOS. Should a match not be found, then EnSight will use all the
settings for the default Configuration but substitute the name specified by '-c name' for the hostname.
The Job Launch Configuration Setting dialog lists entries by a 'Configuration name' which can be different than the
'Hostname'. The Hostname must be a properly routable intranet/Internet hostname and/or TCP/IP address. A
Configuration name can be any name that doesn't include spaces or special characters. The configuration name and
hostname can be identical.

Network ports used by EnSight and SLiM
Client/Server Mode
The EnSight client connects to the slimd8 license manager via TCP port 7790 typically. This actual port used is
defined in $CEI_HOME/license8/slim8.key and appears on the 'slimd' line as the number after 'slimd'.
The client listens for connections from the EnSight server on TCP port 1106. It also communicates with the
collaborative hub on TCP port 1107. If the client is listening for external commands, it will use TCP port 1104.
If port 1106 is used by another process, EnSight will give you an error "Address already in use", and there are two
possible solutions:
1: use another port with command line option "-ports ####" for both client and server (inconvenient)
2: kill (or have root kill) the process that has the port locked.
For example, determine the process:
/sbin/fuser 1106/tcp
the result comes back....
1106/tcp: 314159o
in this case you(or root, if necessary) would kill it...
kill -9 314159
Note that the specific commands to use will vary depending on operating system.
Server of Server Mode
When running in Server of Server mode (SOS), the SOS is threaded and will start up server processes in parallel
(subject to CPU availability and license restrictions) using ports 1110 through 1117. To limit the number of threads,
set the environmental variable ENSIGHT9_MAX_SOSTHREADS to the maximum number of threads (max is 8).

Page 20

Distributed Renderer - used by parallel compositor
Ports 8739 to 8789 must be available to EnSight for its own internal TCP/IP connections when running the parallel
compositor in EnSight DR.

SEE ALSO
Chapter 2 of the Getting Started Manual
How To Load Multiple Datasets (Cases)

Page 21

Command Line Start-up Options

INTRODUCTION
There are a number of options that can be included on the command line when starting EnSight. The following tables
indicate the commands that can be issued for the EnSight script (ensight92), the EnSight client (ensight92.client), the
EnSight server (ensight92.server), or the EnSight server-of-servers (ensight92.sos). To see the most current listing
for any of these, issue one or more of the following:
Linux/Unix/Mac
ensight92 -help
ensight92.client -help
ensight92.server -help
ensight92.sos -help

Windows
ensight92_client -help
ensight92_server -help
ensight92_sos -help

BASIC USAGE
ensight92 [options]
or

ensight92.client [options]
Section 1. EnSight Startup/Client-Server Options
-ar 
Restore from specified archive file “f”
-c [[:]]
Do an auto connection, with optional “host” machine and executable. If only -c is used, the
auto connection will be according to the values set in your ensight_conn_settings file (which is
created in your EnSight Defaults directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at
C:\Users\username\ on Vista and Win7, C:\Documents and Settings\yourusername\ on older
Windows, ~/.ensight92 on Linux, and in ~/Library/Application Support/EnSight92 on the Mac) if
you connect via the Connect dialog). EnSight server will run on “host” if you include it after

-case 
-cierr
-cip

-cm
-collab_port <#>
-ctx 
-custom
-cwd 

-d #
-display #
-delay_refresh
-extcfd
-externalcmdport
-externalcmds

-gold
-hide_console
-homecwd
-lite
-localhostname 
-no_delay_refresh
-p 

the -c. And you can also optionally specify the server executable to run on said “host”.
Read EnSight casefile name ”f” and display part loader
Connect auto and ignore errors
Send client’s IP address to the server for auto connect. The IP address will be used
instead of the internet hostname. This can be useful for clients which use dynamic IP
address assignment (i.e. dhcp). (However, it may not send the correct address if the
client computer has multiple network interfaces (e.g. WiFi and wired ethernet).)
Do a manual connection of server
Specify the port for collaboration socket communication.
Applies context file “f” as soon as connection is made
Force the license manager to look for a custom token
Sets the client working directory to the path specified by ‘p’
Command line display?
Graphics window is not updated during command file playback, until finished
Extended CFD variables automatically placed in variable list
Specify the port on which to receive external commands. See -externalcmds.
Has EnSight start listening for a connection on port 1104 (or the port specified with the
-externalcmdport) for an external command stream. Once connected, all commands
must then come from the external source - as the GUI commands will be ignored.
Force the license manager to look for a gold token
(Windows only) hides console on startup
(Windows only) Sets the client working directory to HOME
Start EnSight in Lite mode
Host name to force server(s) to use to connect to client
Graphics window is updated during command file playback, until finished
Plays playfile “f” as soon as connection is made

Page 22

-part_loader

If a file is specified on the command line, this command will bring up the part loader to
allow for part selection. If a file is specified on the command line without this command,
all parts will be loaded.
-ports #
Allows user specification of socket communication port. (passed on to server or sos)
-prdist #
Specify a parallel rendering distribution config file.
-pyargv . . . [-endpyargv] Anything on the command line between these two options will appear as ‘sys.argv’ in
Python. sys.argv[0] = “ensight” except if a python startup file is specified via -qtguipy, in
which case, that filename becomes sys.argv[0]. Note, -pyargv will swallow arguments
up to the end of the argument list or -endpyargv, whichever comes first.
-rsh 
Remote shell program to use for automatic connection. (passed on to server or sos)
-security [#]
Forces a handshake between the client and server using the # provided or a random
number
-sos
Set up to connect to the Server-of-Servers (ensight92.sos) instead of normal server.
-soshostname 
Host name to force server(s) to use to connect to Server-of-Servers
-standard
Force the license manager to look for a standard token
-timeout <#>
Number of seconds to wait for server connection; default = 60, infinite = -1
-token_try_again <#>
If can’t obtain a license token, try again in # minutes. where # is a float value. If neither
-token_wait_for nor -token_wait_until is specified, will try for 1 hour.
-token_wait_for #
If can’t obtain a license token, try again for # minutes, where # is a float value.
If -token_try_again is not specified, sets -token_try_again to 10.
Supersedes -token_wait_until.
-token_wait_until #
If can’t obtain a license token, try again until the time is hour:minute. If -token_try_again
is not specified, sets -token_try_again to 10.
-v #
Output verbosity 0 to 10
-version
Prints out EnSight’s version number. (Does not start EnSight)
Section 2. EnSight Client GUI Options
-E
Call a method on a registered user-defined extension (see EnSight extension
mechanism and How to Produce Customized Access to Tools & Features) using
the name of the extension. There must be no space between the -E and the extension
name and the option can be used repeatedly in the same command line (the order of
execution matches the order on the command line). These calls are made just prior to
playing command files or python files after EnSight starts up. By default, the method
‘cmdLine()’ is invoked, but options exist to specify the method as well as parameters to
the method. The whole option may need to be enclosed in quotes if some of these latter
features are used.
For example, suppose you have a registered extension named ‘foo’. The following
usages are permitted.
‘-Efoo’ will call foo.cmdLine().
‘-Efoo.run()’ will call foo.run(), a specific object method.
‘-Efoo=10.0’ will call foo.cmdLine(10.0), the default method with a parameter.
‘-Efoo.bar(10.0,”hello”)’ will call foo.bar(10.0, “hello”), a specific object method with
multiple parameters.
-iconlblf <#>
Mode panel icon label font size
-ignorexerr
Ignore X window errors
-jumboicons
Adds support for high resolution displays such as IBM Big Bertha (linux/unix) (see -mag)
-largeicons
Uses larger feature icons in EnSight (non-Windows only)
-mag #
Magnification factor of menus, titlebars, icons using a float number that is greater than
1.0 on high resolution displays or power wall (Windows only).
-menuf #
Menu font size (4 to 50)
-ni
Will use text in place of icons
-sc 
Section Label color name “c” string < 24 chars long
-smallscreen
Sets window attributes based on the screen size of 1024x768 (non-Windows only)
-smallicons
Uses smaller feature icons in EnSight (default)
Section 3. EnSight Server Specific Options

Page 23

-buffer_size <#>
-gdbg
-iwd
-maxoff
-no_ghosts
-no_metric
-readerdbg
-scaleg <#>
-scalev <#>
-swd 

-time
-writerdbg

Set element buffer size for Unstructured Auto Distribute (passed from client down)
Print some debugging info for EnSight format geometries (passed from client to server)
Ignore the working directory in the ensight.connect.default file
Turns off maxsize checking (passed from client to server)
Don’t produce ghosts in Unstructured Auto Distribute (passed from client down)
Don’t print metric for Unstructured Auto Distribute (passed from client down)
Prints user-defined-reader library loading information in shell window upon startup of
server (passed from client to server)
Provide scale factor to scale geometry by (passed from client to server)
Provide scale factor to scale all vectors by (passed from client to server)
Set the server working directory
Prints out timing information (passed from client to server)
Prints user-defined-writer library loading information in shell window upon startup of
server (passed from client to server)

Section 4. Miscellaneous Options
-h, -help, -Z
Prints the usage list
-inputdbg
Prints user-defined input device information
-nb
No automatic backup recording
-no_file_locking
Turns off file locking (lock()). Some systems don’t support this properly
-no_prefs
Do not load saved user preferences (uses all original defaults)
-pal_tex
Use 1D textures for color palettes.
-pal_rgb
Use rgb colors for color palettes
-range10
Use palette ranges which are 10% in from the extremes
-silent
Causes all stdout and stderr messages to be thrown away
-slimtimeout #
Allow slimd token to expire if idle.
-stderr 
Cause all stderr messages to be written to the file.
-stdout 
Causes all stdout messages to be written to the file.
Section 5. Rendering Options
-batch < height> Batch mode with optional width and height.
-bbox
Render only bounding boxes in the GUI window (useful for detached displays with
-prsd2 option). (See How To Setup For Parallel Rendering)
-box_resolution <#>
Resolution of bounding boxes for part culling (max 9). Implies -no_display_list
-ctarget <#>
Set the number of chunks per server for parallel rendering (passed from client to
server(s)).
-dconfig
Specify a display configuration file
-display_list
Use OpenGL display lists
-frustrum_cull
Use frustrum culling where possible
-glconfig
Prints current OpenGL configuration parameter defaults to screen
-glsw
Forces use of software implementation of OpenGL, bypassing the hardware graphics
card (same as -X)
-gl
Sets line drawing mode to draw polygons
-ogl
Sets line drawing mode to draw lines
-no_display_list
Force EnSight to use immediate mode graphics
-no_frustrum_cull
Do not use frustrum culling
-norm_per_vert
Use one normal per vertex for flat-shading
-norm_per_poly
Use one normal per polygon for flat-shading
-multi_sampling
Turns MultiSampling on
-multi_sampling_sw
Use software MultiSampling
-no_multi_sampling
Do not use MultiSampling
-no_start_screen
Ignore the start screen image (Good for HP using TGS OpenGL)
-num_samples <#>
Specify number of samples for software multi-sampling
-num_samples_st <#>
Specify number of samples for hardware stereo multi-sampling
-occlusion_test
Use the HP occlusion extension if available

Page 24

-no_occlusion_test
-stencil_buff
-no_stencil_buff
-double_buffer
-single_buffer
-sort_first
-sort_last
-unmapdd
-vcount <#>

-X

Do not use the HP occlusion extension
Use the OpenGL stencil buffer (even if not enabled by default)
Assumes there is not a working stencil buffer (some Windows video cards)
Use double-buffering for the graphics window (default)
Do not use double-buffering
Sets the default parallel rendering sorting method to be the sort first method
Sets the default parallel rendering sorting method to be the sort last method
Don’t map the detached display on startup
Specifies the maximum number of vertices between begin/end pairs in a OpenGL
display list object. This option is useful for certain graphics cards (most modern Nvidia
based) when dealing with large display objects - it will usually impact the performance of
creating the display list objects. Every graphics card/driver will be optimal at a different
vcount value so testing is necessary to achieve maximum performance.
Starts the X version of EnSight (uses Mesa OpenGL instead of native OpenGL,
bypassing the hardware graphics card. This is the same as -glsw)

Section 6. X Window Specific Options
-bg 
Background “color” colorname, such as “white”
-fg 
Foreground “color” colorname, such as “black”
-fn 
(UNIX only) Motif GUI font where “fn” is the XLFD font name
-font 
Same as -fn
-hc 
User Interface Current Selection Highlight “color” colorname, such as “yellow”.
Section 7. Resource Options
-chres 
Collab hub resource filename
-res 
Resource filename
-sosres
SOS resource filename
-use_lsf_for_renderers
Evaluate environmental variable LSB_MCPU_HOSTS for renderer resources
(See Client Resources in How To Use Resource Management)
-use_lsf_for_servers
Evaluate environmental variable LSB_MCPU_HOSTS for server resources
(See Client Resources in How To Use Resource Management)
-use_pbs_for_renderers Evaluate environmental variable PBS_NODEFILE for renderer resources
(See Client Resources in How To Use Resource Management)
-use_pbs_for_servers
Evaluate environmental variable PBS_NODEFILE for server resources
(See Client Resources in How To Use Resource Management)
Section 8. Distributed Rendering (DR) Specific Options
-cr
Chromium mode
-offscreen
Batch offscreen rendering
-onscreen
Batch onscreen rendering
-pc
Compositing mode
-pr_out 
File name for parallel rendering worker output

Client Examples:
ensight92 -cm -p myplayfile
This will allow the user to do a manual connection, after which the “myplayfile” will be run.
ensight92 -c -gold -ports 1310 -case myfile.case
This will do an automatic connection (according to information in the user’s ensight.connect.default file) on port 1310,
using a gold seat. After the connection is made, the “myfile.case” casefile will be run.
ensight92 -rsh ssh -hc yellow

(or ensight92.client -c -rsh ssh -hc yellow)

This will use ssh as the remote shell for an automatic connection, and will set the highlight color to yellow (instead of
the default color of green).

Page 25

ensight92.server [options]
-buffer_size <#>
-c 
-ctarget <#>
-ctries <#>
-ether
-gdbg
-h, -help
-maxoff
-no_ghosts
-no_metric
-pipe
-ports <#>
-readerdbg
-scaleg <#>
-scalev <#>
-security <#>
-sock
-soshostname 
-time
-writerdbg

Set element buffer size for Unstructured Auto Distribute
“host” indicates where the client is running
Set the number of chunks per server for parallel rendering.
The number of times (1 second per try) to try to connect client and server.
Ethernet device name such as ln0
Print some debugging info for EnSight format geometries
Prints the usage list
Turns off maxsize checking
Don’t produce ghosts in Unstructured Auto Distribute
Don’t print metric for Unstructured Auto Distribute
Forces the server to use a named pipe connection (must be on same machine)
Allows user specification of socket communication port.
Prints user-defined-reader lib loading information in shell window upon startup of server
Provide scale factor to scale geometry by
Provide scale factor to scale all vectors by
Provide number for client to server security check or else random token is generated
Forces the server to use a socket connection
Allows different name for servers to connect back to Server-of-Servers with
Prints out timing information
Prints user-defined-reader lib loading information in shell window upon startup of server

Server Examples (when started manually):
ensight92.server -c clientmachine -readerdbg
Specifies “clientmachine” as the machine on which the client is running, and that information on user-defined-reader
library loading should be printed out.
ensight92.server -ports 1310 -scaleg 10.0 -scalev 10.0
Specifies that communication is to occur on port 1310, and that the geometry and all vectors are to be scaled by a
factor of 10.

ensight92.sos [options]
-buffer_size <#>
-c 
-cports
-ctarget <#>
-ctries <#>
-ether
-gdbg
-h, -help
-maxoff
-no_ghosts
-no_metric
-pipe
-ports <#>
-readerdbg
-rsh 
-scaleg <#>

Set element buffer size for Unstructured Auto Distribute (passes on to servers)
“host” indicates where the client is running
Allows specification of socket communication port to the client.
See also -ports, -sports.
Set the number of chunks per server for parallel rendering (passes on to servers).
The number of times (1 second per try) to try to connect client and server.
Ethernet device name such as ln0
Print some debugging info for EnSight format geometries (passes on to servers)
Prints the usage list
Turns off maxsize checking (passes on to servers)
Don’t produce ghosts in Unstructured Auto Distribute (passes on to servers)
Don’t print metric for Unstructured Auto Distribute (passes on to servers)
Forces the server to use a named pipe connection (must be on same machine) (passes
on to servers)
Allows user specification of socket communication port. (passes on to servers)
Has the effect of setting -cports and -sports to be the same.
Prints user-defined-reader library loading information in shell window upon startup of
server (passes on to servers)
Remote shell program to use for automatic connection of servers. (passes on to servers)
Provide scale factor to scale geometry by (passes on to servers)

Page 26

-scalev <#>
-security <#>
-slog 
-sock
-soshostname 
-sports
-time
-writerdbg

Provide scale factor to scale all vectors by (passes on to server)
Provide number for client to server security check (passes on to servers)
Create SOS log file ‘f’
Forces the server to use a socket connection
Allows different name for servers to connect back to Server-of-Servers with (passes on
to servers)
Allows specification of socket communication port to the servers.
See also -ports, -cports.
Prints out timing information (passes on to servers)
Prints user-defined-reader library loading information in shell window upon startup of
server (passes on to servers)

SOS (Server-of-Servers) Examples (when started manually):
ensight92.sos -c clientmachinename -soshostname sosmachinename
Specifies “clientmachinename” as the machine on which the client is running, and that the individual servers should
connect back to “sosmachinename”.
ensight92.sos -readerdbg -gdbg
Specifies that the sos and any servers print out user-defined-reader library loading information, and that the servers
print out EnSight data format geometry loading information.

Page 27

Use Environment Variables

INTRODUCTION
There are a number of environment variables that can be set to control and modify aspects of EnSight. These are
generally described in sections of the documentation where they apply. However, for convenience, a summary of
them is indicated below. All, except those indicated otherwise, are optional.
Note: None of the environment variables associated with specific user defined readers and writers are included here.
See the appropriate README files or other documentation for each reader/writer.

BASIC USAGE
List sorted by Category:
Name

Locatio Category
n

Description

ENSIGHT9_COLLABHUB_SPAWNDELAY

Collab

DR

ENSIGHT9_HUB_APP

Collab

DR

ENSIGHT9_HUB_ARGS

Collab

DR

ENSIGHT9_HUB_CONNBACKHOST

Collab

DR

ENSIGHT9_HUB_HOST

Client

DR

ENSIGHT9_HUB_OUTPUTFILE

Collab

DR

ENSIGHT9_RENDERER_HOSTS

Client/
Collab

DR

ENSIGHT9_WORKER_APP

Collab

DR

ENSIGHT9_WORKER_ARGS

Collab

DR

ENSIGHT9_WORKER_CONNBACKHOST

Collab

DR

Delay time (in seconds) between spawning distributed
rendering clients
the executable name for the collabhub when used with
distributed rendering
a string of arguments passed to the collabhub executable
when used with distributed rendering
the hostname that the collabhub should use for the computer
where the main client executes
the hostname that the client should use for the collabhub if
not specified by other means.
a file name containing the output from the collabhub when
used with distributed rendering
a space delimited string consisting of the hostnames to use
for distributed rendering clients. See current client
documentation as well. Also see the Resources
documentation for additional information
the executable name for the client when used with distributed
rendering
a string of arguments passed to the distributed rendering
client executable
the collabhub executable hostname (used by distributed
rendering clients)

CEI_FONT_GLYPHCACHESIZE

Client

Font

CEI_FONT_NOSYSTEMFONTS

Client

Font

CEI_FONTPATH

Client

Font

ENSIGHT_FONT_DEFAULT_ANNOT
ENSIGHT_FONT_DEFAULT_ANNOT_STYLE
ENSIGHT_FONT_DEFAULT_OUTLINE
ENSIGHT_FONT_DEFAULT_OUTLINE_SCALE

Client
Client
Client
Client

Font
Font
Font
Font

ENSIGHT_FONT_DEFAULT_OUTLINE_STYLE
ENSIGHT_FONT_DEFAULT_SYMBOL
ENSIGHT_FONT_DEFAULT_SYMBOL_STYLE
ENSIGHT9_FIXED_FONT_SIZE

Client
Client
Client
Client

Font
Font
Font
Font

CEI_ENABLE_PBUF
CEI_ENABLE_PMAP
CEI_PIXELFORMAT
CEI_PIXELFORMAT_ST
CVF_NO_WM_OVERRIDE

Client
Client
Client
Client
Client

Graphics
Graphics
Graphics
Graphics
Graphics

ENSIGHT_PICK_SCALE

Client

Graphics

Number of font characters to keep in memory at a given time
(default 500). Increasing this number will use more memory
but may increase rendering speed if many different
characters are in use.
Disable the loading of fonts from the system directories, and
use only the fonts provided by CEI.
A list of ":" separated directories (";" on Windows) where
EnSight looks for .ttf and .ttc font files.
Specify family to be used for annotation defaults
Specify style to be used for annotation defaults
Specify family to be used for ID and axis defaults
Specify the relative scale for the outline font. (The value 100.0
is the default, 200.0 is 2x larger, 50.0 is 1/2 size).
Specify style to be used for ID and axis defaults
Specify family to be used instead of the symbol font
Specify style to be used with the symbol font
defines font size - expecting range between 10 and 100 (old)
Enable/disable the use of pbuffers for off-screen rendering
Enable/disable the use of pixmaps for off-screen rendering
Specify pixel format for mono rendering
Specify pixel format for stereo rendering
Change the behavior of detached displays so that the
'OverrideRedirect' attribute is not used on the Windows.
If > 1, modifies the scaling of the GL viewport

Page 28

Name

Locatio Category
n

CEI_RSH

Client/
SoS
Client/
Server
Client/
SoS/
Server

CVF_COMM2_NAGLE
ENSIGHT9_SOCKBUF

Description

Networking Alternative to default ssh command
Networking

Enable Nagle (RFC896) network feature (on by default).

Networking

Sets socket buffer size (can be different between client and
server)

DISPLAY

Client

Other

Do not remote the display from a different machine as this is
inefficient and prone to problems. Run the client on your local
machine and the server remotely and connect them as
EnSight is optimized for this configuration.

ENSIGHT9_MAX_CTHREADS

Client

Parallel

ENSIGHT9_MAX_SOSTHREADS

SoS

Parallel

ENSIGHT9_MAX_THREADS

Server

Parallel

The maximum number of threads to use for each EnSight
client. Threads in the client are used to accelerate sorting of
transparent surfaces. If not defined, then the EnSight client
chooses the number of threads based on the number of
processors available and license limitations.
The maximum number of threads to use on the server of
server in order to start up server processes in parallel rather
than serially. If not defined, then EnSight chooses the number
of threads based on the number of processors available and
license limitations.
The maximum number of threads to use for each EnSight
server. Threads are used to accelerate the computation of
streamlines, clips, isosurfaces, and other compute-intensive
operations. If not defined, then the EnSight server chooses
the number of threads based on the number of processors
available and license limitations.

ENSIGHT9_RES

Client/
SoS/
Collab
Client/
SoS

Resources

Specify a resource file name that the client reads

Resources

LSB_MCPU_HOSTS

Client/
SoS

Resources

Specify quoted strings of space delimited host names (e.g.
“host1 host2 host1 host3”) to be used for EnSight servers.
The host names are used in the order they occur. A host
name may occur multiple times
If either the ‘-use_lsf_for_servers’ or ‘use_lsf_for_renderers’ command line options are
specified, then the client will evaluate this environment
variable for resources. The environment variable specifies a
quoted string such as “host1 5 host2 4 host3 1” which
indicates 5 CPUs should be used on host1, 4 CPUs should be
used on host2, and 1 CPU should be used on host3. The
hosts will be used in a round-robin fashion.

CEI_ARCH

All

Path

CEI_HOME

All

Path

Description of hardware & OS (set automatically on EnSight
startup)
Location of EnSight installation (required)

CEI_PDFREADER

Client

Path

Application for reading EnSight .pdf help files

CEI_PYTHONHOME

Client

Path

CEI_UDILPATH

Client

Path

ENSIGHT_PATHREPLACE

Client

Path

PATH

Path

TMPDIR

Client
Server

Point to a different Python runtime library. Default is
CEI_HOME/apex12/machines/CEI_ARCH/Python242
A list of ":" separated directories (";" on Windows) where
EnSight looks for user-defined image libraries.
Replaces the data path with the path found in this
environment variable
Must include $CEI_HOME/bin

Path

Location for temporary files. Default is usually /tmp or /usr/
tmp

CEI_CONTROLLER_KEY

Client

Tracking

See CEI_INPUT

ENSIGHT9_SERVER_HOSTS

Page 29

Name

Locatio Category
n

Description

CEI_INPUT

Client

Tracking

CEI_TRACKD_DEBUG

Client

Tracking

CEI_TRACKER_KEY

Client

Tracking

To specify the tracking library. To select trackd, use:
setenv CEI_INPUT trackd (for csh or equivalent users)
The value of CEI_INPUT can either be a fully-qualified path
and filename or simply the name of the driver, in which case
EnSight will load the library libuserd_input.so from directory:
$CEI_HOME/apex21/machines/$CEI_ARCH/udi/
$CEI_INPUT/
For the trackd interface you will also need to set:
CEI_TRACKER_KEY 
CEI_CONTROLLER_KEY 
Turn on debug information from the trackD user defined input
library.
See CEI_INPUT

ENSIGHT9_INPUT

Client

Tracking

Input device to use for EnSight (same as CEI_INPUT)

ENSIGHT9_READER

Server

User

Path to the location of additional user-defined readers

ENSIGHT9_READER_GUI

Server

User

ENSIGHT9_UDMF

Server

User

ENSIGHT9_UDW

Server

User

Set to 0 in order to not load user-defined extra GUI. Any other
setting (or unset) loads extra GUI.
Sets directory location of user defined math functions to be
loaded by EnSight at startup
Sets directory location of user defined writers to be loaded by
Ensight at startup

Page 30

Use MPI

INTRODUCTION
EnSight includes support for MPI (Message Passing Interface; see http://www.mcs.anl.gov/research/projects/mpich2/
) for use between EnSight's Server-of-Servers (SOS) application and EnSight Servers (server). Note that EnSight
still has the same SOS support as previous versions of EnSight; MPI support is in addition to previous capabilities.
The user should note that MPI support is an evolving area for EnSight. In particular CEI Inc. is still determining the
best method to distribute the various components related to MPI, how best to support varying MPI implementations
and job schedulers, and the type and degree of support required by end-users. This documentation will be updated
at a future date. Please contact EnSight support if you desire to use MPI with EnSight.

Page 31

Page 32

Page 33

Page 34

Page 35

Read and Load Data
Read Data

INTRODUCTION
EnSight supports a number of file formats common in computational analysis. In addition, CEI has defined generic
data formats (in both ASCII and binary versions) that can be used for both structured and unstructured data. In many
cases analysis codes output this data directly (i.e. FLUENT, STAR-CD, KIVA, etc.)
Reading data into Ensight can be a one-step quick process if an association is
known for the data format type and you wish to load all parts.
A two-step process is also available. This is the more traditional method for
EnSight, and provides more control over the reading of data files and the part
creation process. The first step is the selection of appropriate files. The second step
is the loading of parts. Both steps have many similarities regardless of the data
format. These basic steps are described below. Variations from the methods shown
will be described in Chapter 2 (Reader Basics) of the User Manual for the various
formats. Both of these methods are accessed under File->Open...
One-Step Quick Method (Simple Interface)
One-Step Quick Method (Advanced Interface/Load All)
Ensight_reader_extension.map file example:
Two-Step Method (Advanced Interface/Choose Parts)
First Step (Specifying Files):
Second Step (Loading Parts):

BASIC OPERATION
One-Step Quick Method (Simple Interface)
The one-step method of reading data into EnSight works for most formats and requires a file extension-to-reader
mapping file (ensight_reader_extension.map). This file can reside in the site_preferences directory and/or each user
can have his own personal one in his personal EnSight defaults directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older Windows, and ~/.ensight92 on Linux,
and in ~/Library/Application Support/EnSight92 on the Mac). A sample of this file is shown below. The mapping file
associates file extensions to readers. If this file is not provided or an association is not known, or the format doesn’t
allow it due to required intermediate information (such as Plot3D currently), the one-step method (Simple Interface)

Page 36

will default to the first step of the two-step method (Advanced Interface)
1. Select File > Open...
2. If not already selected, toggle
Simple Interface on.
3. Navigate to the desired directory
using typical navigation methods.
4. Filter the list using the File type, if
desired.
5. Select the desired file.
This file’s extension is what will be
mapped to a reader in the
ensight_reader_extension.map.
6. Click Okay
(Double clicking the file in step 4. is
also allowed.)

At this point (provided the association is successful and the data is readable) all parts of the model will be loaded
into EnSight and will appear in the graphics screen and in the Parts List. If the association is not successful, an
error message will result.

One-Step Quick Method (Advanced Interface/Load All)
A variation of the one-step method of reading data into EnSight can also use the Advanced interface and the Load All
button. The extension-to-reader mapping file (ensight_reader_extension.map) is also used for this variation - but if no
mapping is set, the user can specify the format manually. Note also that this method gives you more control over

Page 37

other format and time options.
1. Select File > Open...
2. If not already selected, toggle
Advanced Interface on.
3. Navigate to the desired
directory using typical
navigation methods.
4. Filter the list using the File
type, if desired.
5. Select the desired file.
This file’s extension is what will
be mapped to a reader in the
ensight_reader_extension.map.
6. Click appropriate Set Button.
If a mapping is known, the correct
Format will be automatically
chosen for you.
7. Select the correct Format - if
not already correct.
8. Click Load All.

At this point (provided the settings are correct) all parts of the model will be loaded into EnSight and will appear in
the graphics screen and in the Parts List. Otherwise an error message will result.

Format options and Time options are documented in the next section.

Page 38

Ensight_reader_extension.map file example:
The following is a sample containing associations for EnSight Case, EnSight5, STL and MSC/Dytran:
EnSight file extension to format association file
Version 1.0
#
# Comment lines start with a #
#
#
# The format of this file is as follows:
#
# READER_NAME: reader name as it appears in the Format chooser in the EnSight Data Reader dialog
# NUM_FILE_1: the number of file_1_ext lines to follow
# FILE_1_EXT: the extension that follows a file name minus the “.”, i.e., “geo”, “case”, etc.
#
There should be one definition after the :. Multiple FILE_1_EXT lines may exist
# NUM_FILE_2: the number of file_2_ext lines to follow
# FILE_2_EXT: the extension of a second file that will act as the result file. This is only used
#
for formats that require two file names. As with FILE_1_EXT, there may be multiple
#
FILE_2_EXT lines.
# ELEMENT_REP: A key word that describes how the parts will be loaded (all parts will be loaded the
#
same way). One of the following:
#
“3D border, 2D full”
#
“3D feature, 2D full”
#
“3D nonvisual, 2D full”
#
“Border”
#
“Feature angle”
#
“Bounding Box”
#
“Full”
#
“Non Visual”
#
If option is not set then 3D border, 2D full is used
# READ_BEFORE: (optional) The name of a command file to play before reading the file(s)
# READ_AFTER: (optional) The name of a command file to read after loading the parts
# Definition for Case files
READER_NAME: Case
NUM_FILE_1: 2
FILE_1_EXT: case
FILE_1_EXT: encas
ELEMENT_REP: 3D feature, 2D full
# Definition for EnSight5 files
READER_NAME: EnSight 5
NUM_FILE_1: 2
FILE_1_EXT: geo
FILE_1_EXT: GEOM
NUM_FILE_2: 2
FILE_2_EXT: res
FILE_2_EXT: RESULTS
ELEMENT_REP: 3D feature, 2D full
# Definition for STL files
READER_NAME: STL
NUM_FILE_1: 4
FILE_1_EXT: stl
FILE_1_EXT: STL
FILE_1_EXT: xct
FILE_1_EXT: XCT
ELEMENT_REP: 3D feature, 2D full
# Definition for Dytran files
READER_NAME: MSC/Dytran
NUM_FILE_1: 2
FILE_1_EXT: dat
FILE_1_EXT: ARC
ELEMENT_REP: 3D border, 2D full
READ_AFTER: read_after_dytran.enc

Page 39

Two-Step Method (Advanced Interface/Choose Parts)
First Step (Specifying Files):
Each data format requires a different set of files for proper data loading. A table is provided below that briefly
describes these files for various formats. Links to the User Manual are also provided - so you can get detailed
information for each format
1. Select File > Open...
2. Toggle Advanced Interface, if not
already set.
3. Navigate to the desired directory
using typical navigation methods.
4. Filter the list using the File type, if
desired.
5. Select the desired file.
This file’s extension is what will be mapped
to a reader in the
ensight_reader_extension.map.

6. Click the applicable Set Button(s)
(in this case, the Set d3plot button)
If a mapping is known, the correct Format
will be automatically chosen for you.

7. Select the correct Format - if not
already correct.
The list shown is dependent on the
presence of internal and user-defined
readers at your site, and in your preference
settings. For the list of available readers
please see Native EnSight Format
Readers or Other Readers.

8. Optionally set any Format
options.
Note the options presented will vary
according to the data format. All but the
Casefile format will allow input of measured
data. See EnSight5 Measured/Particle
File Format. Plot3d, Casefile, and Special
HDF5 structured formats will provide a field
for a boundary file. See EnSight
Boundary File Format

9. Optionally set any Time options.
If desired, specify a starting time. The
default is the last time step, unless you
have set a preference otherwise.

10. Click Choose Parts.

Page 40

The Data Part Loader dialog for the applicable format will now open and you are ready for the second step in the data
reading process.
There are a couple of exceptions to this, where additional information must be entered. For example, the Plot3D
reader requires some confirmation on various formatting possibilities, the ESTET reader allows for vector building
from scalar components, etc. If not obvious, please see the details for specific readers in Chapter 2 (Other Readers)
of the User Manual
Second Step (Loading Parts):
There are several ways that parts are specified for loading into EnSight. Many formats use similar procedures, while
a few have custom methods. Below we present the more common part loading methods. For formats that vary from
these - you will be referred to the User Manual which gives the details for each.
To build unstructured parts for EnSight Case (Ensight Gold, EnSight6), EnSight5, ABAQUS_ODB, Medina bif/bof,
Ansys Results (v8), AVUS, AVUS Case, CFF, CFX-4, CGNS, ExodusIIgold, Special HDF5, LS-DYNA3D, MSC/
Dytran, Nastran OP2, NetCDF, RADIOSS_4.x, SCRYU, Silo, TECPLOT 7.x, Tecplot_ASCII, Vectis, and any other
User-defined formats:
1. If the Data Part Loader dialog is not open,
select File > Load parts...
The available parts are listed in the Parts List. You can build
them all by clicking Load All at the bottom. Alternately, you
can build the selected ones or even one by one and choose a
different visual representation and part name for each.

To build selected parts:
2. Select the desired part(s) in the Parts list.
3. Choose the desired initial Visual
Representation for the select part(s).
Optionally, you can have each of the elements indicated by
the visual rep be represented as a point and a normal.

4. Toggle on if you want the selected parts to be
grouped together.
If on, the “New part description” field will be used as
the group name.

5. If desired, enter a name for the part (to use in
the Main Parts list).
The default name is the same as the entry in this
Parts List.

6. Click Load Selected.
7. Click Close when done.
Note that you can re-enter the part loader and build more parts later for formats which use this method.

Page 41

For ANSYS RESULTS, FAST UNSTRUCTURED, FIDAP NEUTRAL, FLUENT UNIVERSAL, Movie, and MPGS 4.1
formats:
All parts defined in the file will be loaded to the EnSight
server. However, you have a choice for the initial visual
representation of some parts as displayed on the client. The
choice is made with the Load pull-down:
All Parts: all parts are loaded to the client in the default visual
representation (typically 3D Border, 2D Full).
Part 1 Only: Only the first part is loaded to the client in the default
visual representation. The other parts will have the NonVisual
representation.
All But Part 1: All parts other than part 1 are loaded to the client in
the default visual representation. Part 1 will be NonVisual.
No Parts: No parts are loaded to the client (i.e. the representation of
all parts is set to NonVisual).

Note that you can easily change the visual representation of
a part at any time. See How To Change Visual
Representation for more information.
1. Select the desired Load option.
2. Click Okay.
Note that you will not be able to re-enter the part loader for formats which use this method
For the N3S format, see N3S Reader
For the Abaqus_fil format all parts are automatically loaded.

Page 42

To build structured parts for EnSight Case (EnSight Gold, EnSight6), Special HDF5, Plot3D, and any other Userdefined formats:
1. If the Data Part Loader dialog is not
open, select File > Load parts...
2. Be sure Structured Data is selected to
display only the structured parts in the
Parts List.
3. Select the desired part(s) in the Parts
List.

4. Choose the desired initial Visual
Representation for the select part(s).
Optionally, you can have each of the elements
indicated by the visual rep be represented as a point
and a normal.

5. If the selected part has Iblanking, you
can build based on the value (Inside
selects cells where Iblank=1, Outside
selects Iblank=0, All selects all cells
ignoring Iblanking).
6. You can specify From, To, and Step IJK
values for the selected part(s). The From
and To values are inclusive.
Valid values in the From and To fields are numbers
advancing from 1(the min for each part), or numbers
decreasing from 0(the max for each part):
1,2,3,... --->
<--- ...-3,-2,-1,0
|-------------------------------------------|
min
max
(always 1)
(varies per part)
If you specify values that will be outside of the range
of an individual part, the proper min or max values
for the given part will be used.

The Min and Max fields are for reference only.
8. If desired, enter a name for the part (to
use in the Main Parts list). The default
name is the same as the entry in the
Parts List.
9. Open this turndown section to create
unstructured parts based on boundary
Iblanking from any parts created above.

7. If you desire to extract multiple
surfaces (at a constant delta) from the
same zone, set one of the directions to
the desired non-zero delta value.
This is a “blade row” kind of operation.
Please note that this results in an
unstructured part instead of a structured one.

10. Click Create/load from selected.
(or Create/load all if you want to load all the
structured parts)

11. Click Close when done.
For the ESTET format the procedure is similar. See ESTET Reader

Page 43

SEE ALSO
How To Use ens_checker
User Manual:
Reader Basics
EnSight Case Reader
EnSight5 Reader
Other Readers

Page 44

Page 45

Use ens_checker

INTRODUCTION
This program attempts to check the integrity of the EnSight Gold (or EnSight6) file formats. Most files that pass this
check will be able to be read by EnSight (see Other Notes below). If EnSight Gold (or EnSight6) data fails to read into
Ensight, one should run it through this checker to see if any problems are found.
Ens_checker makes no attempt to check the validity of floating point values, such as coordinates, results, etc. It is
just checking the existence and format of such.

BASIC OPERATION
Program invocation:
If you invoke the program without any arguments, it will prompt you for the casefile to read. For example:
> ens_checker
*****************************************************************
* EnSight Data Format Checker
*
* ===========================
*
*
Currently,
*
*
1. Must be run from directory in which casefile is located. *
*
2. Handles EnSight6 and EnSight Gold formats only.
*
*
3. Does not process SOS casefiles.
*
*****************************************************************
 mydata.case

You can alternatively invoke the program with the casefile on the command line.
> ens_checker mydata.case

Sample runs:
As ens_checker works it will be providing feedback. This feedback is important in interpreting what is wrong in the
files. Here is a sample run, which was successful:
> ens_checker 3by3.case
*****************************************************************
* EnSight Data Format Checker
*
* ===========================
*
*
Currently,
*
*
1. Must be run from directory in which casefile is located. *
*
2. Handles EnSight6 and EnSight Gold formats only.
*
*
3. Does not process SOS casefiles.
*
*****************************************************************
 3by3.case
Casefile to Process:
-------------------3by3.case
(Opened successfully)
--------------------Major Sections Found:
--------------------Required FORMAT
section
Required GEOMETRY section
Optional VARIABLE section
Optional TIME
section
--------------FORMAT Section:
--------------EnSight 6 Format

(at
(at
(at
(at

line
line
line
line

1)
4)
7)
11)

(set at line 2)

Page 46

------------TIME section:
------------Info for timeset number: 1
---------------------------Time set: 1
(at line 12)
No description provided
Number of steps:
1
(at line 13)
Time values:
(starting on line 14)
time values[1] = 0
>-------------------<
> TIME section OKAY <
>-------------------<
----------------GEOMETRY Section:
-----------------------Model filename is:

3by3.geo

(at line 5)

Static geometry
-------Opened 3by3.geo successfully
File type is:
Description 1:
Description 2:
node ids:
element ids:

ASCII
EnSight test geometry file
==========================
assign
assign

Global section:
Number of nodes: 64
Coordinates for (64) nodes found
Part 1:
Description is: 3 x 3 xy
Unstructured Part
Number of quad4 elements is: 9
Connectivities for (9) quad4 elements found
Part 2:
Description is: 3 x 3 yz
Unstructured Part
Number of quad4 elements is: 9
Connectivities for (9) quad4 elements found
Part 3:
Description is: 3 x 3 xz
Unstructured Part
Number of quad4 elements is: 9
Connectivities for (9) quad4 elements found
Part 4:
Description is: 3 x 3 45
Unstructured Part
Number of quad4 elements is: 9
Connectivities for (9) quad4 elements found
>-----------------------<
> GEOMETRY section OKAY <
>-----------------------<
----------------VARIABLE Section:
----------------scalar per node:
scalar
Filename is: 3by3.scl
Non transient variable

(at line 8)

Page 47

-------Opened 3by3.scl successfully
Description: 3by3 scalar variable
Global section:
(64) Nodal scalar values for unstructured nodes found
vector per node:
vector
Filename is: 3by3.vct
Non transient variable

(at line 9)

-------Opened 3by3.vct successfully
Description: 3by3 vector variable
Global section:
(192) Nodal vector values for unstructured nodes found
>-----------------------<
> VARIABLE section OKAY <
>-----------------------<
>----------- Hooray! ----------<
>
<
> Data verification SUCCESSFUL <
>
<
>
with No Warnings
<
>
<
>------------------------------<

And here is a sample run, with a problem, namely a ‘block’ line is missing:
> ens_checker 3by3s.case
*****************************************************************
* EnSight Data Format Checker
*
* ===========================
*
*
Currently,
*
*
1. Must be run from directory in which casefile is located. *
*
2. Handles EnSight6 and EnSight Gold formats only.
*
*
3. Does not process SOS casefiles.
*
*****************************************************************
Casefile to Process:
-------------------3by3s.case
(Opened successfully)
--------------------Major Sections Found:
--------------------Required FORMAT
section
Required GEOMETRY section
Optional VARIABLE section
Optional TIME
section
--------------FORMAT Section:
--------------EnSight 6 Format

(at
(at
(at
(at

line
line
line
line

1)
4)
7)
11)

(set at line 2)

------------TIME section:
------------Info for timeset number: 1
----------------------------

Page 48

Time set: 1
(at line 12)
No description provided
Number of steps:
1
(at line 13)
Time values:
(starting on line 14)
time values[1] = 0
>-------------------<
> TIME section OKAY <
>-------------------<
----------------GEOMETRY Section:
-----------------------Model filename is:

3by3s.geo

(at line 5)

Static geometry
-------Opened 3by3s.geo successfully
File type is:
Description 1:
Description 2:
node ids:
element ids:

ASCII
EnSight test geometry file
==========================
assign
assign

Global section:
Number of nodes: 0
Part 1:
Description is: 3 x 3 xy block
Structured Part
Not iblanked
i j k = 4 4 1
Number of nodes: 16
Number of cells: 9
Block X coordinates for (16) nodes found
Block Y coordinates for (16) nodes found
Block Z coordinates for (16) nodes found
Part 2:
Description is: 3 x 3 yz block
===> Problem:
------------Looking for one of the following valid line types:
element type
(unstructured types, any of the following:
point
tria6
tetra10
penta15
bar2
quad4
pyramid5
hexa8
bar3
quad8
pyramid13
hexa20
tria3
tetra4
penta6
block
(structured block)
part
(the next part)
but found the following:
4
4
1
>-------------------------<
> GEOMETRY section FAILED <
>-------------------------<
>-*-*-*-*-*-* bummer! *-*-*-*-*-*-<
>
<
> Verification of the data FAILED <
>
<
>-*-*-*-*-*-*-*-*-*-*-*-*-*-*-*-*-<

After fixing the ‘block’ line and running the program again, another problem is encountered - namely, an extra space
Page 49

at the end of the second line of x coordinates for the block that is part 2.
> ens_checker 3by3s.case
*****************************************************************
* EnSight Data Format Checker
*
* ===========================
*
*
Currently,
*
*
1. Must be run from directory in which casefile is located. *
*
2. Handles EnSight6 and EnSight Gold formats only.
*
*
3. Does not process SOS casefiles.
*
*****************************************************************
Casefile to Process:
-------------------3by3s.case
(Opened successfully)
--------------------Major Sections Found:
--------------------Required FORMAT
section
Required GEOMETRY section
Optional VARIABLE section
Optional TIME
section
--------------FORMAT Section:
--------------EnSight 6 Format

(at
(at
(at
(at

line
line
line
line

1)
4)
7)
11)

(set at line 2)

------------TIME section:
------------Info for timeset number: 1
---------------------------Time set: 1
(at line 12)
No description provided
Number of steps:
1
(at line 13)
Time values:
(starting on line 14)
time values[1] = 0
>-------------------<
> TIME section OKAY <
>-------------------<
----------------GEOMETRY Section:
-----------------------Model filename is:

3by3s.geo

(at line 5)

Static geometry
-------Opened 3by3s.geo successfully
File type is:
Description 1:
Description 2:
node ids:
element ids:

ASCII
EnSight test geometry file
==========================
assign
assign

Global section:
Number of nodes: 0
Part 1:
Description is: 3 x 3 xy block
Structured Part
Not iblanked
i j k = 4 4 1
Number of nodes: 16

Page 50

Number of cells: 9
Block X coordinates for (16) nodes found
Block Y coordinates for (16) nodes found
Block Z coordinates for (16) nodes found
Part 2:
Description is: 3 x 3 yz block
Structured Part
Not iblanked
i j k = 4 4 1
Number of nodes: 16
Number of cells: 9
===> Problem:
------------Previous lines end with 1 extra chars on the line,
but line 2 has 2 extra chars. The lines must be consistent
or EnSight will have trouble reading it.
===> Problem:
------------Not successful reading 16 X block coordinates
>-------------------------<
> GEOMETRY section FAILED <
>-------------------------<
>-*-*-*-*-*-* bummer! *-*-*-*-*-*-<
>
<
> Verification of the data FAILED <
>
<
>-*-*-*-*-*-*-*-*-*-*-*-*-*-*-*-*-<

After eliminating the extra space, the file then checked out fine.

ADVANCED USAGE
Redirecting Output to a File:
ens_checker is writing to stderr, so if you want to redirect output to a file, you need to use “>&”. For example, the
following will place the output of the run into a file called output.file:
> ens_checker 3by3.case >& output.file

OTHER NOTES
The word “most” is used above because one of the things that could pass the checker, but fail in EnSight is element
connectivity of EnSight6 files with node ids. The ens_checker checks that node ids used in the element connectivities
lie within the min and max range of the node ids, but does not verify that there is actually a node with each individual
id.
The validity of model extents, presence of nan’s, etc. are currently checked to some degree in ens_checker, but
again, this is a format checker - not a model integrity checker.

SEE ALSO
User Manual:
EnSight Gold Casefile Format
EnSight6 Casefile Format

Page 51

Load Multiple Datasets (Cases)

INTRODUCTION
Normal operation of EnSight involves one client process (the graphics and GUI) interfacing with one server process
(data I/O and computation) to postprocess your data. There however several other configurations possible. One of
these is the ability to connect a single client to multiple servers at the same time, with each server maintaining a
unique dataset. Each of these servers can potentially run on different machines.

Server

Client
Normal Operation

Server

Server

Client
Two Cases

The main use of this capability is to visualize multiple datasets simultaneously. Each dataset is loaded into a separate
case and can be viewed in the same window or in separate viewports. You can perform before and after comparisons
of the same problem or compare experimental with simulated results. The same operation (such as a clip or a particle
trace) can be performed in both cases simultaneously. Created parts always belong to the same case as the parent
from which the part was created. As a consequence, you cannot perform operations that combine parts (such as a
merge) from multiple cases.
When EnSight reads a new case, it searches the current list of variables for matches with the variables from the new
case. If it finds a match (based on an exact match of the variable name), it will not enter the new variable in the list.
Rather, the matched name will be used for both. This behavior is based on the assumption that the identical variable
names represent the same physical entity and should therefore be treated the same. If the new variable name does
not match any existing name, the new variable is added to the list as usual.
Up to 16 cases can be active at one time. You can add a new case or replace an existing case to a running session
by using the File->Open... process (if you want to load all parts and don’t need to control other options available when
loading cases) or the File->Data (reader)... process (which provides greater control). Adding a case starts a new
server process, connects it to the client, and either loads all the parts (if you used Open...) or allows you to specify the
data format and files as well as which parts to load into the new server and what optional settings to use as the case
is created. One of the helpful uses of the replace case option is to load a new dataset into EnSight without re-starting
the client. You can of course also delete cases you no longer need.

Page 52

BASIC OPERATION
Simplified case operations (Add or Replace and load all parts) can be accessed through the File->Open dialog. All
other case operations (including control of various options can be accessed through the Case menu or through the
File->Data (reader) dialog. Both methods will be shown below.

Add a Case
To add a case to a running EnSight session
Using simple File->Open dialog
method:
1.Select File->Open... to open
the File Selection dialog.

2. Select Keep currently loaded
data
This will add, rather than
replace, the case

3. Select the desired directory
and files for the new case.
4. Click Okay.

The EnSight client will now start the connection process for the new server. If your original connection was
automatic, the new server will be started automatically. If your original connection was manual, you will have to
manually start another server. You can follow the progress of the connection in the Message area. See the
EnSight Getting Started Manual or How To Connect EnSight Client and Server for more information. Once
connected, EnSight will also load all parts of this new case if you use this method.

Page 53

Using File->Data (reader) dialog method:
1. Select Case > Add, Replace, Delete... to open the data reader File Selection dialog.

2. If the Case section is not
open, click the turndown.
3. Click Add...

4. If desired, enter a name for the
case (other than the default).
The name will be displayed in the
Case menu so this case can be
selected as the current case.
5. Set optional settings.
Create new viewport for this case will
place the new case in a new viewport.
Apply Context From Case 1 will cause
the new case to inherit positioning etc.
from case 1.
Reflect Model About Axis allows the
model to be reflected as it is read in.
Pick the axis and specify the origin
location.
6. Click Okay.
The EnSight client will now start the connection process for the new server. If your original
connection was automatic, the new server will be started automatically. If your original connection
was manual, you will have to manually start another server. You can follow the progress of the
connection in the Message area. See the EnSight Getting Started Manual or How To Connect
EnSight Client and Server for more information.

Page 54

Replace a Case
You can replace an existing case. This is most useful when you wish to load a new dataset without having to stop
and re-start the client. To replace a case:
Using simple File->Open dialog method:
Do the same thing you do for adding a case, but select the Replace currently loaded data toggle.
Using File->Data (reader) dialog method
1. Select the case you wish to replace in the Case menu (Case > casename).
2. Select Case > Add, Replace, Delete... to open the data reader File Selection dialog.
3. If the Case section is not open, click the turndown.
4. Click Replace...
You will be asked to confirm the replacement. If confirmed, the server associated with the selected case is terminated
and the EnSight client will now start the connection process for the new server. If your original connection was
automatic, the new server will be started automatically. If your original connection was manual, you will have to
manually start another server. You can follow the progress of the connection in the Message area. See How To
Connect EnSight Client and Server for more information.

Delete a Case
To delete a case:
1. Select the case you wish to delete in the Case menu (Case > casename).
2. Select Case > Add, Replace, Delete... to open the data reader File Selection dialog.
3. If the Case section is not open, click the turndown.
4. Click Delete...
You will be asked to confirm the deletion. If confirmed, the server associated with the selected case is terminated.

Displaying Parts by Case
By default all parts from all cases are displayed in the Main Parts list and they are displayed in a hierarchical manner
by case. There are several different ways to show or not show things in the list. These are controlled by the Sort...
button under the list. See How To... Introduction to Part Creation for more details on viewing the parts list.

Page 55

Case Viewport Display
One of the chief advantages of the case feature is the ability to perform side-by-side comparisons of different
datasets. One way to do this is to display each case in a separate viewport. To do this:
1. Create as many additional viewports as you need to
display your cases. See How To Define and Change
Viewports for more information.
2. Select the case whose parts you wish to display only in
certain viewports in the Case menu (Case > casename).
3. Select Case > Viewport Visibility...
4. Click in the desired viewport to enable or disable
display of the selected case. Black means the selected
case is not displayed in the viewport, green means that
it is displayed.

ADVANCED USAGE
EnSight’s cases capability has also been used to achieve coarse-grained parallelism for very large datasets by
partitioning a mesh into blocks and reading each block into a different case. Each case can run on different machines
or on different CPUs of a multiprocessor host. Since the EnSight client places the geometry from the different cases
in the same coordinate system, the blocks are effectively “stitched” back together for viewing. Operations such as
clipping and isosurface calculation are then automatically performed in parallel. However, since there is no
communication between the servers (in the current release) you cannot trace particles originating in one block and
expect them to cross a block boundary into a different block. (It should be noted that EnSight’s server-of-server
capability is an alternate, and usually better way to do parallel operations on a model.)

OTHER NOTES
When you perform an archive operation, a binary dump file is produced for each active server (case). The archive
information file contains details about the cases and can be used to restart the EnSight client as well as all servers
active when the archive was performed. See How To Save and Restore an Archive for more information.

SEE ALSO
User Manual: Case Menu Functions

Page 56

Load Transient Data

INTRODUCTION
From it’s inception, EnSight has been used extensively to postprocess time-varying or transient data. In many cases,
dynamic phenomena can only be understood through interactive exploration as a transient case is animated.
EnSight handles all types of transient data. All variables as well as mesh coordinates and connectivity can vary over
time. The rate at which variables (or the mesh) change can differ (supported through the EnSight Gold and EnSight6
Case data format only).
EnSight can postprocess transient data in many ways. The Solution Time Quick Interaction area lets you easily set
the current time step, step through time (manually or automatically), or restrict the range of time to a region of
interest. You can perform query operations to extract information over time. You can use the flipbook capability to
create an on-screen animation of your data changing over time and continue to interact with it during animation
playback. EnSight’s keyframe animation capability can be used to create high-quality video animations of transient
data.
This article covers reading transient data into EnSight.

BASIC OPERATION
Reading transient data into EnSight is essentially the same as reading static data (see How To Read Data for more
information). By default, the last time step will become the current time step. This behavior is based on the
assumption that the last step will contain the largest dynamic range of the variable data so that variable palettes will
be initialized properly. However, you can override this by clicking the Specify Starting Time Step toggle and entering
the desired time step in the data reader File Selection dialog (File > Data (Reader)...).
For most data formats, the “results” file supplies the necessary time information, including number of steps, actual
solution time at each step, and how to access the dynamic variable and geometry files. However, some formats
supported by EnSight include this information in the same file that contains other geometry or variable data. The
following table lists how transient data is specified for each format type. And for the latest and most detailed
information, please look at the README file in the reader folder under $CEI_HOME/ensight92/src/readers.
Format Type
Case

What File Contains Time Info?

Notes

EnSight 6

file.case

Standard EnSight case file

EnSight Gold

file.case

Standard EnSight case file

EnSight 5

file.res

Standard EnSight results file

ABAQUS

file.fil

ABAQUS_ODB

file.odb

ANSYS RESULTS

file.rst, file.rth, etc.

Ansys Results (v8)

file.rst, file.rth, etc.

AVUS

Does not handle transient data directly

AVUS Case

file.txt

CFF

file

CFX-4

file.dmp

CGNS

file.cgns

ESTET

AVUS text case file

Does not handle transient data

ExodusIIgold

file.exo

FAST UNSTRUCTURED

file.res. Can handle transient geometry
as well as solution and function files.

Special FAST format results file. See FAST
UNSTRUCTURED Results File Format

FIDAP NEUTRAL

file.fdneut

All time steps must be contained in the same neutral
file (i.e. there is only one file, not one for every time
step).

Fluent

file.cas, file.dat

FLUENT UNIVERSAL

file.unv

Special FLUENT format results file. See FLUENT
UNIVERSAL Results File Format

Page 57

Format Type

What File Contains Time Info?

Notes

Special HDF5

file (each file contains one time value)

Special casefile containing number of files and the list
of files to use.

LS-DYNA3D

file.d3plot

Can be all in one file or in a family of d3plot files.

Medina bif/bof

file.konfig

Movie

file.res

Standard EnSight results file

MPGS 4.1

file.res

Standard EnSight results file

MSC/Dytran

file.arc files

Remember file.dat can be used to assemble multiple
“parts” from multiple file.arc files.

Nastran OP2

file.op2

N3S

file.res

NetCDF

file.ncase

PLOT3D

file.res. Can handle transient geometry
as well as solution and function files.

RADIOSS_4.x

file.anim

SCRYU

file.pre

Silo

file.silo or file.case

STL

N3S results file

Special PLOT3D format results file. See PLOT3D
Results File Format.

Multiple times can be in the file.silo file, or the
file.case file can contain reference to multiple files
and their times.
Does not handle transient data

TECPLOT 7.x

file.plt

Tecplot_ASCII

file.dat for single file transient
or file*.dat (file1.dat, file2.dat, etc.)

For a single file transient solution, use
SOLUTIONTIME=# keyword after each ZONE T
keyword where # is a number representing the time
and check the Single File Transient Toggle in the
Format Options Tab of the data reader.
For multiple files, use file*.dat where the * represents
the file number of the timestep.

Vectis
Other User Defined

varies with each reader

See How to Read User Defined

SEE ALSO
How To Change Time Steps, How To Animate Transient Data, How To Query/Plot
User Manual: Flipbook Animation, Query/Plot

Page 58

Use Server of Servers

INTRODUCTION
ensight92 (with gold license key) has the capability of dealing with partitioned data in an efficient distributed manner
by utilizing what we call a server-of-servers (SOS for short). An SOS server resides between a normal client and a
number of normal servers. Thus, it appears as a normal server to the client, and as a normal client to the various
normal servers.

This arrangement allows for distributed parallel processing of the various portions of a model, and has been shown to
scale quite well.
Currently, EnSight SOS capability is only available for EnSight5, EnSight6, EnSight Gold, Plot3d, and any EnSight
User-Defined Reader data. (It is not directly available for Fidap Neutral, Fluent Universal, N3S, Estet, MPGS4,
Movie, Ansys, Abaqus, or FAST Unstructured data.)
Please recognize that your data must be partitioned in some manner (hopefully in a way that will be reasonably load
balanced) in order for this approach to be useful. (The exception to this is the use of the auto_distribute capability for
structured or unstructured data. This option can be used if the data is available to all servers defined. It will
automatically distribute each portion of the data over the defined servers - without the user having to partition the
data. If you also use “resources”, a SOS casefile is not even needed. Please note that currently only EnSight
Gold, Plot3d, and any 2.06 (or greater) user-defined readers (which have implemented structured reader
cinching) can be used for structured auto_distribute - and that only EnSight Gold and any 2.08 (or greater)
user-defined readers (which have implemented the “*_in_buffers” routines ) can be used for unstructured
auto_distribute.)
(Included in the EnSight distribution is an unsupported utility that will take most EnSight Gold binary unstructured
datasets and partition it externally for you. The source for this utility (called “chopper”) can be found in the
$CEI_HOME/ensight92/unsupported/partitioner directory.)
Note: If you do your own partitioning of data into EnSight6 or EnSight Gold format, please be aware that each part
must be in each partition - but, any given part can be “empty” in any given partition. (All that is required for an empty
part is the “part” line, the part number, and the “description” line.)
You should place each partitioned portion of the model on the machine that will compute that portion. Each
partitioned portion is actually a self contained set of EnSight data files, which could typically be read by a normal
client - server session of EnSight. For example, if it were EnSight gold format, there will be a casefile and associated
gold geometry and variable results file(s). On the machine where the EnSight SOS will be run, you will need to place
the sos casefile. The sos casefile is a simple ascii file which informs the SOS about pertinent information needed to
run a server on each of the machines that will compute the various portions.
Page 59

The format for this file is as follows: (Note that [ ] indicates optional information, and a blank line or a line with # in the
first column are comments.)
FORMAT
type: master_server datatype

(Required)
(Required)
where:

datatype is required and is one of the formats of EnSight’s internal readers (which
use the Part builder), namely:
gold

ensight6

ensight5

plot3d

or it can be the string used to name any of the user-defined readers.
Note: For user-defined readers, the string must be exactly that which is defined in the
USERD_get_name_of_reader routine of the reader (which is what is presented in the Format
pulldown of the Data Reader dialog).
If datatype is blank, it will default to EnSight6 data type.
[auto_distribute: on/off]

(Optional for structured or unstructured data)
EnSight will automatically distribute data to the servers specified below if this option is present
and set to “on”. This will require that each of the servers have access to the same data (or
identical copies of it). For structured data: use only if the datatype is gold, plot3d or a 2.06
or greater user-defined reader (which has implemented structured cinching). For
unstructured data: use only if the datatype is gold, or a 2.08 (or greater) user-defined
reader. Additionally, be aware that 2.* user-defined readers should implement the special
functions defined in README_USERD_IN_BUFFERS file if memory is to be used efficiently in
the unstructured auto-distribute process.

[use_resources: on/off]

(Optional, to allow specification of server machines to come from the “resource file”)

[plot3d_iblanked:
true/false]
(Required only if doing auto_distribute and datatype is plot3d)
[plot3d_multi_zone:
true/false]
(Required only if doing auto_distribute and datatype is plot3d)
[plot3d_dimension:
1d/2d/3d]
(Required only if doing auto_distribute and datatype is plot3d)
[plot3d_source: ascii/cbin/fortranbin](Required only if doing auto_distribute and datatype is plot3d)
[plot3d_grid_double: true/false]
(Required only if doing auto_distribute and datatype is plot3d)
[plot3d_results_double: true/false] (Required only if doing auto_distribute and datatype is plot3d)
where: iblanking, multi_zone, dimension, source type, grid file double precision, and results file
double precision information should be provided. If it is not provided, it will default to the
following (which is likely not to be correct):
plot3d_iblanked:
plot3d_muti_zone:
plot3d_dimension:
plot3d_source:
plot3d_grid_double:
plot3d_results_double:

false
false
3d
cbin
false
false

[do_ghosts:

on/off]

(Optional for unstructured auto_distribute - default is on)
Allows user to control whether ghost cells will be produced between the distributed portions.

[buffer_size:

n]

(Optional for unstructured auto_distribute and do_ghosts - default is 100000)
Allows user to modify the default buffer size that is used when reading node and element
information of the model when producing ghost cells.

[want_metric:

on/off]

(Optional for unstructured auto_distribute and do_ghosts - default is on)
If set on, a simple metric will be printed in the shell window that can indicate the quality of the
auto_distribution. The unstructured auto_distribute method relies on some coherence in the
element connectivity - namely, that elements that lie next to each other are generally listed close
to each other in the data format.
The metric is simply the (#total_nodes / #nodes_needed_if_no_ghosts).
When no ghosts, the value will be 1.0. The more ghosts you must have, the higher this metric
will be. If the number gets much more than 2.0, you may want to consider partitioning yourself.

NETWORK_INTERFACES

(Note: This whole section is optional. It is needed only when more than one network
interface to the sos host is available and it is desired to use them. Thus, distributing the servers
to sos communication over more than one network interface)

Page 60

number of network interfaces: num(Required - if section used)
where: num is the number of network interfaces to be used for the sos host.
network interface: sos_network_interface_name_1(Required - if section used)
network interface: sos_network_interface_name_2(Required - if section used)
.
.
network interface: sos_network_interface_name_num(Required - if section used)

SERVERS
(Required)
number of servers: num [repeat](Required)
where: num is the number of servers that will be started and run concurrently.
repeat indicates that the first server specification should be repeated num times for use
with resources. Other server specifications will be ignored.
#Server 1
machine id: mid

(Comment only)
(Required)
where: mid is the machine id of the server.

executable: /.../ensight92.server(Linux/Unix/Apple Required, must use full path)
or ensight92_server.bat
(Windows only Required, must use .bat extension)
[directory: wd]
(Optional)
where: wd is the working directory from which ensight92.server will be run
[login id: id]

(Optional)
where: id is the login id. Only needed if it is different on this machine.

[data_path: /.../dd]

(Optional)
where: dd is the directory where the data resides. Full path must be provided if you use this line.

casefile: yourfile.case

(Required, but depending on format, may vary as to whether it is a casefile, geometry file,
neutral file, universal file, etc. Relates to the first data field of the Data Reader Dialog.)

[resfile: yourfile.res]

(Depends on format as to whether required or not. Relates to the second data field of the Data
Reader Dialog.)

[measfile: yourfile.mea]

(Depends on format as to whether required or not. Relates to the third data field of the Data
Reader Dialog.)

[bndfile: yourfile.bnd]

(Depends on format as to whether required or not. Relates to the fourth data field of the Data
Reader Dialog.)

--- Repeat pertinent lines for as many servers as declared to be in this file ---

BASIC OPERATION
To use Server of Servers, you must:
1. Partition your data, and distribute it (or make it available) to the various machines on which you will run servers.
(Or if all servers have access to the data, you can use the auto_distribute option in the sos casefile.)
2. Create the sos casefile, which defines the server machines, the location of server executables on those machines,
and the name and location of the [partitioned] data for the servers.
3. Use ensight92.sos in place of ensight92.server, and provide it with the sos casefile.

Example SOS Casefile
This example deals with a EnSight Gold dataset that has been partitioned into 3 portions, each running on a different
machine. The machines are named joe, sally, and bill. The executables for all machines are located in similar
locations, but the data is not. Note that the optional data_path line is used on two of the servers, but not the third.
FORMAT
type: master_server gold
SERVERS
number of servers: 3
#Server 1
machine id: joe
executable: /usr/local/bin/ensight92/bin/ensight92.server

Page 61

data_path: /usr/people/john/data
casefile: portion_1.case
#Server 2 is a Windows machine (notice .bat extension)
machine id: sally
executable: C:\Program Files\CEI\ensight92\bin\ensight92_server.bat
data_path: D:\john\data
casefile: portion_2.case
#Server 3
machine id: bill
executable: /usr/local/bin/ensight92/bin/ensight92.server
casefile: /scratch/temp/john/portion_3.case

If we name this example sos casefile - “all.sos”, and we run it on yet another machine - one named george, you would
want the data distributed as follows:
On george:
On joe (in /usr/people/john/data):
On sally (in /scratch/sally/john/data):
On bill (in /scratch/temp/john):

all.sos
portion_1.case, and all files referenced by it.
portion_2.case, and all files referenced by it.
portion_3.case, and all file referenced by it.

By starting EnSight with the -sos command line option (which will autoconnect using ensight92.sos instead of
ensight92.server), or by manually running ensight92.sos in place of ensight92.server, and providing all.sos as the
casefile to read in the Data Reader dialog - EnSight will actually start three servers and compute the respective
portions on them in parallel.
So, one could do the following (after preparing the all.sos file):
On “george”, run the client and the sos by invoking the ensight92 script in a shell window (non-windows) or
Command Prompt window (windows), like:
george>> ensight92 -sos
Or one could run the client on the “myclient” machine, telnet (or equivalent) into the “george” machine and run the sos
there, by using the following commands:
If “myclient” is a non-windows machine:
In a window on “myclient”:

In a window that is telneted into the “george” machine:

myclient>> ensight92.client -cm

If “george: is a non-windows machine:
george>> ensight92.sos -c myclient
If “george is a windows machine:
george>> ensight92_sos -c myclient

:
If “myclient” is a windows machine:
In a Command Prompt window on “myclient”:

In a Command Prompt window that is telneted into the
“george” machine:

myclient>> ensight92_client -cm

If “george: is a non-windows machine:
george>> ensight92.sos -c myclient
If “george is a windows machine:
george>> ensight92_sos -c myclient

In either case, you would enter the all.sos command as the file to read in the Data Reader dialog once EnSight is up
and connected. And the servers on “joe”, “sally”, and “bill” would be started and used automatically.

Page 62

ENVIRONMENT Variables
The following Environment variables will directly affect the SOS performance, see How To Setup for Parallel
Computation.
ENSIGHT9_MAX_THREADS
ENSIGHT9_MAX_SOSTHREADS
Optional NETWORK_INTERFACES section notes
If the machine named george had more than one network interface (say it had its main one named george, but also
had one named george2), we could add the section shown below to our casefile example:
NETWORK_INTERFACES
number of network interfaces: 2
network interface: george
network interface: george2

This would cause machine joe to connect back to george, machine sally to connect back to george2, and machine bill
to connect back to george. This is because the sos will cycle through its available network interfaces as it connects
the servers. Remember that this is an optional section, and most users will probably not use it. Also, the contents of
this section will be ignored if the -soshostname command line option is used.

Example SOS Casefile for PLOT3D, Using structured auto_distribute
This example shows a plot3d dataset (post.x and post.q) that has not been partitioned, but is on an nfs mounted disk
available to each server machine. EnSight will distribute the data to the 3 servers defined. IO will not necessarily be
great since each server will be reading from the same file, but execution will be enhanced by the partitioning. We will
use the same machines used in the previous example.
FORMAT
type: master_server plot3d
auto_distribute: on
plot3d_iblanked: true
plot3d_multi_zone: false
plot3d_dimension: 3d
plot3d_source: cbin
plot3d_grid_double: false
plot3d_results_double: false
SERVERS
number of servers: 3
#Server 1
machine id: joe
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data
casefile: post.x
resfile: post.q
#Server 2
machine id: sally
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data
casefile: post.x
resfile: post.q
#Server 3
machine id: bill
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data
casefile: post.x
resfile: post.q

Page 63

Example SOS Casefile for EnSight Gold, Using unstructured auto_distribute
This example shows an EnSight Gold dataset (trial.case) that has not been partitioned, but is on an nfs mounted disk
available to each server machine. EnSight will distribute the data to the 3 servers defined. IO will not necessarily be
great since each server will be reading from the same file, but execution will be enhanced by the partitioning. We will
use the same machines used in the previous examples.
FORMAT
type: master_server gold
auto_distribute: on
do_ghosts:
on
buffer_size:
10000
want_metric:
on
SERVERS
number of servers: 3
#Server 1
machine id: joe
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data/gold
casefile: trial.case
#Server 2
machine id: sally
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data/gold
casefile: trial.case
#Server 3
machine id: bill
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data/gold
casefile: trial.case

Special Case:
If using auto_distribute (and thus each server will be accessing the same data files), and the servers will all be run on
the same machine, then one can add the word “repeat” to the end of the “number of servers: num” line and then only
define one set of Server info. For example:
FORMAT
type: master_server gold
auto_distribute: on
SERVERS
number of servers: 3 repeat
#Server 1
machine id: joe
executable: /usr/local/bin/ensight92/bin/ensight92.server
data_path: /scratch/data/gold
casefile: trial.case

Structured Auto Distribute Note:
If using structured auto_distribute, the default decomposition scheme is to do so in the i, j, or k direction that has the
largest dimension. This may not always be the best direction for a given analysis. Thus, through the use of an
environment variable, the user can set the axis to use. The chosen axis will be used unless the dimension in that
direction will not allow for all servers to contain data (namely, as long as the dimension in the chosen direction is
greater than the total number of servers used). To use the this option, set the following to 0, 1, 2, or -1:
setenv SAD_DECOMPOSE_AXIS 0
1
2
-1

(for the i axis)
(for the j axis)
(for the k axis)
(to use the default largest dimension scheme,
same as not setting the variable)

Page 64

SEE ALSO
How To Read Data
How To Read User Defined
How To Setup for Parallel Computation
How To Use Resource Managament
User Manual: Server-of-Server Casefile Format

Page 65

Load Spatially Decomposed Case Files

INTRODUCTION
If one has multiple EnSight gold casefiles (each of which contain a spatially decomposed portion of the same model),
they can be read using one or more servers (as long as the number of servers is less than or equal to the number of
casefiles). In other words, when it is desired to read N casefiles with M servers (M<=N), an additional section can be
added to the SOS casefile to accomplish this. Note that the following important restrictions/limitations will apply:
1. M (number of servers) must be less than or equal to N (number of casefiles).
2. Unstructured data only. (Note: a similar capability exists for structured data. See How to Use Block Continuation)
3. Auto distribute may not be specified in the SOS casefile.
4. None of the following can be specified in the partition casefiles:
GEOMETRY
measured:
match:
boundary:
rigid_body:
Vector_glyphs:
BLOCK_CONTINUATION

MATERIAL

Note: that some of the restrictions (such as measured) may eventually be lifted. But currently all of the above are
in effect.
5. All of the normal SOS requirements still apply.
a) All parts must be present in all cases. (Empty parts are allowed)
b) The same variables must exist in all cases.
c) The same timesets must be used in all cases.
Note: If the desired number of servers is equal to the number of casefiles, one can either use the procedure
described in this How To, or could use the normal SOS procedures (see How To Use Server of Servers).

BASIC OPERATION
To postprocess your partitioned EnSight Gold unstructured data on fewer servers than casefiles, run SOS using an
SOS casefile that has a MULTIPLE_CASEFILES section.
Three possible methods are available for your convenience . They all accomplish the same thing in slightly different
ways. So use whichever is easiest for your situation.
Note: in using one of the 3 the methods below, one should determine something about how the data resides, or is
available to EnSight. Namely, how will one need to specify the path to the data.
Since the whole idea is that the number of servers may vary, and Ensight will determine which casefiles go
to which servers, there are really only two possibilities for paths.
A) There is a global path for all of the data. And thus each server needs to know this global path (which it
will prepend to each casefile).
B) Each casefile has its own path. And each server needs to know the path for each.

Page 66

Available Section lines:

Comments

MULTIPLE_CASEFILES

Required for all methods

total number of cfiles:

n

Used for method 1 and 2

cfiles global path:

global_path

Optional, used for methods 1 and 2

cfiles:

partition_1.case

Used for method 1

partition_2.case
.
.
partition_n.case
cfiles pattern:

partition_*.case

Used for method 2

cfiles start number:

#

Used for method 2

cfiles increment:

#

Used for method 2

cfiles file:

filename

Used for method 3

Example
Method 1
Specify the number of and the actual files in the sos casefile
A) Using global path:
MULTIPLE_CASEFILES
total number of cfiles: 3
cfiles global path: /home/bjn/data
cfiles: file1.case
file_b.case
bruce.case
B) Using path per casefile:
MULTIPLE_CASEFILES
total_number of cfiles: 3
cfiles: /home/bjn/data1/file1.case
/home/bjn/data2/file_b.case
/home/bjn/data3/bruce.case
Method 2
Specify the number of, the pattern, and the start and increment
A) Using global path:
MULTIPLE_CASEFILES
total number of cfiles: 3
cfiles global path: /home/bjn/data
cfiles pattern: file**.case
cfiles start number: 0
cfiles increment: 1
OR
MULTIPLE_CASEFILES
total number of cfiles: 3
cfiles pattern: /home/bjn/data/file**.case
cfiles start number: 0
cfiles increment: 1

Page 67

B) Using path per casefile:
Note: method 2 does not have a way to have a separate path for each casefile.
Method 3
Similar to 1., but place the info in a separate file
A) Using global path:
MULTIPLE_CASEFILES
cfiles file: all_together_cfiles.txt
and in all_together_cfiles.txt, (first line contains number of, second line contains the optional global path, then
filenames come 1 per line on the following lines). Like:
3
/home/bjn/data
file1.case
file_b.case
bruce.case
B) Using path per casefile:
MULTIPLE_CASEFILES
cfiles file: separated_cfiles.txt
and in separated_cfiles.txt, (first line contains number of, second line must be the word “none” - indicating no global
path specified, then filenames come 1 per line on the following lines). Like:
3
none
/home/bjn/data1/file1.case
/home/bjn/data2/file_b.case
/home/bjn/data3/bruce.case

Another Example
An EnSight Gold unstructured transient geometry model with a couple of variables, in 4 partitions, like:
bjn1.case
bjn1.geo0000
bjn1.geo0001
bjn1.scalar0000
bjn1.scalar0001
bjn1.evector0000
bjn1.evector0001

bjn2.case
bjn2.geo0000
bjn2.geo0001
bjn2.scalar0000
bjn2.scalar0001
bjn2.evector0000
bjn2.evector0001

bjn3.case
bjn3.geo0000
bjn3.geo0001
bjn3.scalar0000
bjn3.scalar0001
bjn3.evector0000
bjn3.evector0001

bjn4.case
bjn4.geo0000
bjn4.geo0001
bjn4.scalar0000
bjn4.scalar0001
bjn4.evector0000
bjn4.evector0001

Using Method 1:
If they all reside in the same directory (/home/bjn), a method 1 SOS casefile that will use just 2 servers (perhaps
named bjn_4x2.sos) should look like:
FORMAT
type: master_server gold
MULTIPLE_CASEFILES
total number of cfiles: 4
cfiles global path: /home/bjn
cfiles: bjn1.case
bjn2.case
bjn3.case
bjn4.case
SERVERS
number of servers: 2 repeat

Page 68

machine id:
executable:

gun
ensight9.server

Using Method 2:
If they all reside in the same directory (/home/bjn), a method 2 SOS casefile that will use just 2 servers should look
like:
FORMAT
type: master_server gold
MULTIPLE_CASEFILES
total number of cfiles: 4
cfiles global path: /home/bjn
cfiles pattern: bjn*.case
cfiles start number: 1
cfiles increment: 1
SERVERS
number of servers: 2 repeat
machine id: gun
executable: ensight9.server
Using Method 3:
For this one, lets change things and say that they reside in separate directories, like:
/scratch/portion1
bjn1.case
bjn1.geo0000
bjn1.geo0001
bjn1.scalar0000
bjn1.scalar0001
bjn1.evector0000
bjn1.evector0001

/scratch/portion2
bjn2.case
bjn2.geo0000
bjn2.geo0001
bjn2.scalar0000
bjn2.scalar0001
bjn2.evector0000
bjn2.evector0001

/scratch/portion3
bjn3.case
bjn3.geo0000
bjn3.geo0001
bjn3.scalar0000
bjn3.scalar0001
bjn3.evector0000
bjn3.evector0001

/scratch/portion4
bjn4.case
bjn4.geo0000
bjn4.geo0001
bjn4.scalar0000
bjn4.scalar0001
bjn4.evector0000
bjn4.evector0001

the SOS casefile could look like:
FORMAT
type: master_server gold
MULTIPLE_CASEFILES
cfiles file: /scratch/bjn.txt
SERVERS
number of servers: 2 repeat
machine id: gun
executable: ensight9.server
and the /scratch/bjn.txt file could look like:
4
none
/scratch/portion1/bjn1.case
/scratch/portion2/bjn2.case
/scratch/portion3/bjn3.case
/scratch/portion4/bjn4.case
or could look like: (See the Other Notes below)
4
/scratch
portion1/bjn1.case
portion2/bjn2.case
portion3/bjn3.case
portion4/bjn4.case

Page 69

OTHER NOTES:
When your casefile data resides in separate directories below a parent, such as:
/home/bjn
/home/bjn/data1
/home/bjn/data2
/home/bjn/data3
it is valid to use the global path to specify the parent directory, and the individual files to give the path on down. Such
as:
cfiles global path: /home/bjn
cfiles: data1/file1.case
data2/file_b.case
data3/bruce.case
This will result internally as the same thing as if you had done:
cfiles: /home/bjn/data1/file1.case
/home/bjn/data2/file_b.case
/home/bjn/data3/bruce.case

APPENDED_CASEFILES Variation:
If you desire to use all casefiles on one server, you can obviously do so with the above option by using the SOS with
one server. However, there is a variation on this option that can be used without using the SOS. It can be used with
a client and server alone.
It is very similar to the MULTIPLE_CASEFILES option in an SOS casefile, except that it is placed in the first regular
casefile of the series - the one that you will read. It uses APPENDED_CASEFILES as the section header, and lists
just the additonal casefiles (not the one that this is placed in).
So instead of using the SOS with an SOS casefile like:
FORMAT
type: master_server gold
MULTIPLE_CASEFILES
total number of cfiles: 4
cfiles global path: /home/bjn
cfiles: bjn1.case
bjn2.case
bjn3.case
bjn4.case
SERVERS
number of servers: 1
machine id: gun
executable: ensight92.server
You could place the following in bjn1.case:
FORMAT
type: ensight gold
GEOMETRY
model:
bjn1.geo
VARIABLE
scalar per node:

scalar bjn1.scl

APPENDED_CASEFILES
total number of casefiles: 3
cfiles global path: /home/bjn
cfiles: bjn2.case
bjn3.case
bjn4.case
Note that all current limitations for the MULTIPLE_CASEFILES option (which were enumerated above) also
apply to the APPENDED_CASEFILES option. The two options cannot be used in combination. It is an either

Page 70

or situation.

SEE ALSO
How To Read Data
How To Setup for Parallel Computation
How To Use Resource Management
User Manual: Server-of-Server Casefile Format

Page 71

Read User Defined

INTRODUCTION
EnSight provides a mechanism for users to write their own readers and have the code automatically link and execute
at run-time (using a shared library).This capability is documented in the EnSight Interface Manual. As indicated in
that manual, sample readers, as well as the code for several actual readers are provided below the following
directory: $CEI_HOME/ensight92/src/readers/. In subdirectories underneath, are README files that contain
the latest information on using existing user defined readers.
Also, as explained in that manual, be aware that a udr_checker.c file is provided in $CEI_HOME/ensight92/src/
readers/checker directory. This can be used to debug your User-defined reader before using it with EnSight.

OTHER NOTES
When starting EnSight (ensight92 or ensight92.server), you can use the command line option “-readerdbg” to echo
user defined reader loading status. This will allow you to see what readers are actually being loaded.
Set the environment variable ENSIGHT9_READER to point to the path where additional user defined readers exist
and then start up with the -readerdbg option described above to verify that you are loading the reader(s) of interest.

SEE ALSO
The EnSight Interface Manual, as well as:
How To Read Data

Page 72

Do Structured Extraction

INTRODUCTION
When building parts from the Data Part Loader dialog for structured parts (Ensight6 structured parts, EnSight gold
structured parts, PLOT3D parts), there is some flexibility in what is actually extracted. If the model contains iblanking,
then you have control over which iblanking domain to use, namely Inside, Outside (blanked out), or All (which ignores
the iblanking). If no iblanking in the model, the domain is All by default. You can extract all or portions of zones at
original or coarser resolutions, do the extractions on single or multiple zones, extract planes at every delta value
within a zone, etc.

BASIC OPERATION
When extracting the domain parts, whether iblanked or not, some (but definitely not all combinations) of the options
include:

Extracting a complete zone at original resolution,
1. Select the structured zone desired.
Optionally you can change the domain and provide a part
description.
2. Hit the Create/Load from selected button.
The part will be created and shown in the graphics window.
In the example below, it is shown in border representation
mode.

Page 73

Extracting a complete zone at coarser resolution,
1. Select the structured zone desired.
Optionally you can change the domain and provide a part
description.
2. Modify the Step values.
These should be positive integer values. A step of two means
to deal with every other plane, a step of four means every
fourth plane, etc.
3. Hit the Create/Load from selected button.
The part will be created and shown in the graphics window. In
the example below, it is shown in border representation mode.
Note that it is considerably coarser than the previous because
step values of 2, 4, and 5 were used in the ijk directions
respectively.

Page 74

Extracting portions of a zone,
1. Select the structured zone desired.
Optionally you can change the domain and provide a part
description.
2. Modify the From and To values.
These can be anything between the ranges shown in the
Min and Max columns. By default they will be the entire
range, but you can modify them.
3. Hit the Create/Load from selected button.
The part will be created and shown in the graphics
window. In the example below, it is shown in border
representation mode. Note that you now get a portion
instead of the whole. Note also that we got original
resolution because we set step values back to one. The
step values can be other than one, and your portion will be
at the coarser resolution.

Page 75

Extracting multiple planes within the same zone (these become unstructured),
1. Select the structured zone desired.
Optionally you can change the domain and provide a part
description.
2. Modify the From and To values so that one
dimension is a plane.
One of I, J, or K must have the same values for both From
and To - indicating a plane in the other two dimensions.
3. Enter a value in the Delta field for the dimension that
is a plane.
Only one of the Delta fields may be non-zero, and it must
be one where the From and To values are the same.
4. Hit the Create/Load from selected button.
The part will be created and shown in the graphics
window. In the example below, it is shown in border
representation mode. Note that you now get an IK surface
at J = 1, 6, 11, 16, 21, 26, ...

Page 76

Extracting the same portions over multiple parts,
1. Select the structured zones desired.
Optionally you can change the domain
2. Modify the From and To values.
These can be anything between the ranges shown in the Min
and Max columns (which will now be the min and max of all
parts selected). By default they will be the entire range, but
you can modify them. Additionally, “-1” is a valid entry,
indicating the last plane. Minus numbers are ways to specify
the plane from the max back toward the min, thus -2 equals
the next to last plane. (Note: Zero is treated the same as -1)
3. Hit the Create/Load from selected button or the
Create/load all button.
In this example, 4 parts will be created, and they will each be
the full extent IK plane at J = 1 for each of the four zones.
Note that the IK ranges can actually vary per part because the
max is specified, but each zone may be less than the max.

In our example, we then changed From and To to be “0”, thus
extracting the last plane in each zone. Note the image below.
The image at the right includes complete zones that were
extracted, but shown in feature angle representation so
you get the feel of the complete zone.

Page 77

Extracting unstructured iblanked parts.
1. Select the structured zones desired.
Optionally you can change the Domain, From, To, and
Step values.
2. Hit the Create/Load from selected button.
In this example, 4 parts will be created, and they will each
be the full extents at original resolution. Iblanking for the
domain will be ignored.
3. Open the Iblanked Part Creation turndown.
4. Select from the domain parts that you have
previously created.
5. Select the iblanking value to use.
Optionally you can specify your own name for the part
that will be created.
6. Hit the Create and Load Iblanked Unstructured Part
button.
This will create an unstructured part consisting of the
elements which have the selected iblank value from the
selected parts.

SEE ALSO
How To Read Data
User Manual: Using Node Ranges:

Page 78

Use Block Continuation

INTRODUCTION
Given a situation where structured data blocks have been partitioned for analysis on multiple compute nodes, and the
data can be saved in EnSight Gold format, such that a set of cases exists which are contiguous from one set to
another - the data can be read into Ensight using the casefile Block Continuation capability. This allows any number
of these contiguous sets to be clustered and visualized together in an EnSight server. Furthermore, by using this
capability combined with Ensight’s Server of Servers, one can visualize M number of sets with N number of EnSight
Servers. Where m is greater than n.
Please note that each set must be a standalone EnSight case containing a portion of all the parts. The block parts in
each of the sets must consist of a valid subset range of each complete block part. This will require, for example, that
a given 3D block part will vary in only one dimension throughout the sets. Also, each set must be the neighboring
portion or “slice” in the set of cases. Note the following simple example:
i dir
Block Part 1 advances in the i direction.
Block Part 2 advances in the j direction.
j dir

Each Case (or set) consists of portions of both
parts, which are specified using EnSight’s block
range capability. Thus, the first case has the red
portions. The second case has the yellow
portions, etc.
Each block part can be “sliced up” in a different
direction, but that direction must continue for all
sets for that part. And the sets must be the
contiguous natural neighbors of each other.
Note that the block dimensions must remain the
same in the non-advancing directions, but they
can vary per set in the advancing direction (even
though in this simple example they are quite
consistent).

With data set up like the above, we might then decide that we will visualize the model with only two servers. We could
combine (using Block_Continuation) the first two sets onto the first server and the last 3 sets onto the second server.
Portion of Block Part 1 on server 1
(consists of original sets 1 and 2)

Portion of Block Part 2 on server 1
(consists of original sets 1 and 2)
Portion of Block Part 1 on server 2
(consists of original sets 3, 4, and 5)

Portion of Block Part 2 on server 2
(consists of original sets 3, 4, and 5)

Page 79

BASIC OPERATION
To combine more than one of the sets for a given server (what we may call a “cluster” of sets), one must create a
casefile which contains a Block_Continuation section (as described in Chapter 11 of the User Manual).
In our example on the previous page, there were five case files (with their associated geo and scl files).
set_1.case set_2.case set_3.case set_4.case set_5.case
set_1.geo
set_2.geo
set_3.geo
set_4.geo
set_5.geo
set_1.scl
set_2.scl
set_3.scl
set_4.scl
set_5.scl
and the contents of the first of these casefiles (set_1.case) would look something like:
FORMAT
type: ensight gold
GEOMETRY
model:
set_1.geo
VARIABLE
scalar per node:
set_1.scl

With the contents of each of the other casefiles differing only in the digit following the underscore.
To “cluster” these as described (two sets in the first case and 3 sets in the second case), we would need to create the
following two casefiles.
cluster_1.case, would contain:
FORMAT
type: ensight gold
GEOMETRY
model: set_%.geo
VARIABLE
scalar per node:
set_%.scl
BLOCK_CONTINUATION
number of sets:
2
filename start number: 1
filename increment:
1

Note the use of % as the wildcard for
block continuation sets.

cluster_2.case, would contain:
FORMAT
type: ensight gold
GEOMETRY
model: set_%.geo
VARIABLE
scalar per node:
set_%.scl
BLOCK_CONTINUATION
number of sets:
3
filename start number: 3
filename increment:
1

And we could then easily use an SOS casefile (perhaps named, two_blocks.sos) that would use these two cluster
files:
FORMAT
type: master_server gold
SERVERS
number of servers: 2
#Server 1
machine id: node1
executable: ensight92.server
casefile: cluster_1.case
#Server 2
machine id: node2
executable: ensight92.server
casefile: cluster_2.case

Page 80

If you now run EnSight using this SOS casefile, the two block parts should appear as you would expect. Of course, to
avoid any visual (or computational) effects from the partitioning, you would need to be using ghost cells between the
original partitions (sets). See EnSight Gold Geometry File Format and the example file below.
For a description of block range usage, which the original partition (sets) use in describing the block geometry, See
EnSight Gold Geometry File Format
An example of such is the third set geometry file (set_3.geo), which is using uniform blocks with ranges:
Uniform Block Continuation Test - set 3
=======================================
node id assign
element id assign
extents
0.00000e+00 1.00000e+00
-5.00000e+00 1.00000e+00
0.00000e+00 5.00000e+00
part
1
horizontal
block uniform range
2
2
6
1
2
1
2
0.00000e+00
0.00000e+00
2.00000e+00
1.00000e+00
1.00000e+00
1.00000e+00
part
2
vertical
block uniform range
2
11
2
1
2
5
7
0.00000e+00
-2.00000e+00
0.00000e+00
1.00000e+00
-0.50000e+00
1.00000e+00

3

4

1

2

Curvilinear and rectilinear descriptions for block parts are of course also valid.
This same file using ghost cells is:
Uniform Block Continuation Test - set 3
=======================================
node id assign
element id assign
extents
0.00000e+00 1.00000e+00
-5.00000e+00 1.00000e+00
0.00000e+00 5.00000e+00
part
1
horizontal
block uniform with_ghost range
2
2
6
1
2
1
2
0.00000e+00
0.00000e+00
1.00000e+00
1.00000e+00
1.00000e+00
1.00000e+00
ghost_flags
1
0
1
part
2

2

5

Page 81

vertical
block uniform with_ghost range
2
11
2
1
2
4
0.00000e+00
-1.50000e+00
0.00000e+00
1.00000e+00
-0.50000e+00
1.00000e+00
ghost_flags
1
0
0
1

8

1

2

Transient Example
If we change our example to be a simple transient model, using the same sets, but now with two time steps:
set_1_00.case set_2_00.case set_3_00.case set_4_00.case set_5_00.case
set_1_00.geo
set_2_00.geo
set_3_00.geo
set_4_00.geo
set_5_00.geo
set_1_00.scl
set_2_00.scl
set_3_00.scl
set_4_00.scl
set_5_00.scl
set_1_01.case
set_1_01.geo
set_1_01.scl

set_2_01.case
set_2_01.geo
set_2_01.scl

set_3_01.case
set_3_01.geo
set_3_01.scl

set_4_01.case
set_4_01.geo
set_4_01.scl

set_5_01.case
set_5_01.geo
set_5_01.scl

The contents of the first of these casefiles (set_1_00.case) would now look something like:
FORMAT
type: ensight gold
GEOMETRY
model:
1 set_1_**.geo
VARIABLE
scalar per node:
1 set_1_**.scl
TIME
time set:
1
number of steps:
2
filename start number: 0
filename increment:
1
time values:
0.0 1.0

changing_coords_only

With the contents of each of the other casefiles differing only in the digit following the first underscore.
To “cluster” these as described (two sets in the first case and 3 sets in the second case), we would need to create the
following two casefiles.
cluster_1.case, would contain:
FORMAT
type: ensight gold
GEOMETRY
model:
1 set_%_**.geo
VARIABLE
scalar per node:
1 set_%_**.scl
TIME
time set:
number of steps:
filename start number:
filename increment:
time values:
BLOCK_CONTINUATION
number of sets:
filename start number:
filename increment:

changing_coords_only

1
2
0
1
0.0 1.0
2
1
1

cluster_2.case, would contain:

Page 82

FORMAT
type: ensight gold
GEOMETRY
model:
1 set_%_**.geo
VARIABLE
scalar per node:
1 set_%_**.scl
TIME
time set:
number of steps:
filename start number:
filename increment:
time values:
BLOCK_CONTINUATION
number of sets:
filename start number:
filename increment:

changing_coords_only

1
2
0
1
0.0 1.0
3
3
1

And we could then use the same SOS casefile that we showed in the static example.

SEE ALSO
How To Use Server of Servers
How To Read Data
User Manual: EnSight Gold Geometry File Format

Page 83

Use Resource Management

INTRODUCTION
Resources are used to specify which computers are used for running the various EnSight components, specifically
the Server (ensight92.server), the SOS (ensight92.sos), the CollabHub (ensight92.collabhub), and the distributed
renderers (ensight92.client). If you are running a single client and server on a single computer, you may skip this
document.
Resources are an alternative way to specify these computers compared to SOS case files, PRDIST files, Connection
Settings, and command line options. While these other ways are still valid and take precedence for backwards
compatibility, resources greatly simplify specifying computers in a dynamic network environment. For example, SOS
Case files and PRDIST files no longer need to be edited to reflect the current node allocation from cluster batch
schedulers. Resources coupled with native reader support in the SOS even make SOS Case files unnecessary.
Resources can be specified via command line arguments and environment variables. Resources can be specified
multiple times; precedence rules determine which resources ultimately get used. This allows sites to specify defaults
while allowing those to be overridden.

BASIC OPERATION
Resource Files
Resources can be specified via a resource file. Here is an example of a resource file:
#!CEIResourceFile 1.0
SOS:
host: localhost
SERVER:
prologue: “setup_job”
epilogue: “cleanup_job”
host: server1
host: server2
host: server3
host: server4
COLLABHUB:
host: pc0
RENDERER:
prologue: “setenv DISPLAY :0.0”
#
epilogue:
host: pc1
host: pc2
host: pc2

Resource files must begin with the ‘#!CEIResourceFile 1.0’ line. Afterwards, they may have up to four optional
sections: SOS, SERVER, COLLABHUB, and RENDERER. Each of the four sections contains one or more ‘host:
hostname’ lines. These lines specify which computers to use for the corresponding section. ‘hostname’ must be an
Internet/intranet routable host name or IP address. A given host name may appear on multiple lines within a section
or in different sections. If it appears multiple times within a section, then that host will run multiple instances of the
corresponding EnSight component if needed.
Additionally, each section may have an optional ‘prologue: cmd’ line and/or an optional ‘epilogue: cmd’ line.
These specify a command to execute on each host before and after the corresponding EnSight component. Note that
the cmd string must be quoted, and may include appropriate job backgrounding symbols (e.g. ‘&’).
At version 2.0, the resource file can accept an optional ‘shell:’ line, like:
#!CEIResourceFile 2.0
SOS:
host: bunker
shell: "/usr/local/bin/ssh"

Note the new version number (2.0) and that the shell line string must be double quoted.

Page 84

How to specify resources
Resources can be specified via resource files, environment variables, and command line options. Precedence rules
determine which resources will be used. Basically, the last occurrence of a resource section (e.g. SERVER) will be
used in its entirety. For example, if multiple SERVER resource sections are found, only one will be used as determined
by the precedence rules.
Since the EnSight Client, SOS, and CollabHub start other EnSight processes, they can use resources. The EnSight
Server and distributed renderers do not start other EnSight processes that require resources.
While many ways exist to specify resources, in practice only one or two will be used given the particular user’s
computational environment.

Client Resources
The EnSight client supports the following ways for specifying resources:
1. the ENSIGHT9_RES environment variable;
2. the ENSIGHT9_SERVER_HOSTS environment variable;
3. the ENSIGHT9_RENDERER_HOSTS environment variable;
4. the ‘-use_lsf_for_servers’ command line option;
5. the ‘-use_lsf_for_renderers’ command line option;
6. the ‘-use_pbs_for_servers’ command line option;
7. the ‘-use_pbs_for_renderers’ command line option;
8. the ‘-sosres file_name’ command line option;
9. the ‘-chres file_name’ command line option; and
10.the ‘-res file_name’ command line option.
If multiple resources are specified to the client, then they will be evaluated in the order indicated above with the later
methods taking higher precedence for a given section.
The ENSIGHT9_RES environment variable specifies a resource file name that the client reads.
ENSIGHT9_SERVER_HOSTS and ENSIGHT9_RENDERER_HOSTS specify quoted strings of space delimited host
names (e.g. “host1 host2 host1 host3”) to be used for EnSight servers and distributed renderers, respectively.
The host names are used in the order they occur. A host name may occur multiple times.
If either the ‘-use_lsf_for_servers’ or ‘-use_lsf_for_renderers’ command line options are specified, then
the client will evaluate the environment variable LSB_MCPU_HOSTS for the resources. The environment variable
specifies a quoted string such as “host1 5 host2 4 host3 1” which indicates 5 CPUs should be used on host1,
4 CPUs should be used on host2, and 1 CPU should be used on host3. The hosts will be used in a round-robin
fashion.
If either of the ‘-use_pbs_for_servers’ or ‘-use_pbs_for_renderers’ command line options are specified,
then the client will evaluate the environment variable PBS_NODEFILE for the resources. The environment variable
specifies a filename in which the file contains list of line delimited host names that were allocated by the PBS
scheduler.
The ‘-sosres file_name’ command line option specifies the pathname to a resource file. This file name is passed
to the SOS and processed by it; thus the file name must be accessible and readable by the ensight92.sos process. If
multiple ‘-sosres’ options are specified, only the last will be used.
The ‘-chres file_name’ command line option specifies the pathname to a resource file. This file name is passed
to the CollabHub and processed by it; thus the file name must be accessible and readable by the ensight92.collabhub
process. If multiple ‘-chres’ options are specified, only the last will be used.
The ‘-res file_name’ command line option specifies the pathname to a resource file. This command line option
can be specified multiple times. This might be useful when generating resource files dynamically: a single file might
specify only a particular type of resource (e.g. SERVER or RENDERER). The last occurrence of a particular section
takes precedence when multiple ‘-res’ options are given.
Finally, a resource file may be selected in the File->Open dialog for the SOS to use.

Page 85

SOS Resources
The EnSight SOS supports the following ways for specifying resources:
1.
2.
3.
4.
5.
6.
7.
8.

resources gathered and sent from the client;
the ‘-sosres file_name’ command line option;
the ENSIGHT9_RES environment variable;
the ENSIGHT9_SERVER_HOSTS environment variable;
the ‘-use_lsf_for_servers’ command line option;
the ‘-use_pbs_for_servers’ command line option;
the ‘-res file_name’ command line option; and,
a resource file specified via the File->Open dialog.

If multiple resources are specified to the SOS, then they will be evaluated in the order indicated above with the later
methods taking higher precedence for a given section. However, the SOS only uses SERVER section resources; the
other sections are ignored.
The ‘-sosres file_name’ command line option specifies the pathname to a resource file. If multiple ‘-sosres’
options are specified, only the last will be used.
The ENSIGHT9_RES environment variable specifies a resource file name that the SOS reads.
ENSIGHT9_SERVER_HOSTS specifies a quoted string of space delimited host names (e.g. “host1 host2 host1
host3”) to be used for EnSight servers.
If the ‘-use_lsf_for_servers’ command line option is specified, then the SOS will evaluate the environment
variable LSB_MCPU_HOSTS for the resources. The environment variable specifies a quoted string such as “host1 5
host2 4 host3 1” which indicates 5 CPUs should be used on host1, 4 CPUs should be used on host2, and 1 CPU
should be used on host3. The hosts will be used in a round-robin fashion.
If the ‘-use_pbs_for_servers’ command line option is specified, then the SOS will evaluate the environment
variable PBS_NODEFILE for the resources. The environment variable specifies a filename in which the file contains
list of line delimited host names that were allocated by the PBS scheduler.
The ‘-res file_name’ command line option specifies the pathname to a resource file. This command line option
can be specified multiple times. The last occurrence of a particular section takes precedence when multiple ‘-res’
options are given.
Finally, a resource file may be selected in the File->Open dialog for the SOS to use.

CollabHub Resources
The EnSight CollabHub supports the following ways for specifying resources:
1.
2.
3.
4.
5.
6.
7.

resources gathered and sent from the client;
the ‘-chres file_name’ command line option;
the ENSIGHT9_RES environment variable;
the ENSIGHT9_RENDERER_HOSTS environment variable;
the ‘-use_lsf_for_renderers‘ command line option;
the ‘-use_pbs_for_renderers’ command line option; and,
the ‘-res file_name’ command line option.

If multiple resources are specified to the CollabHub, then they will be evaluated in the order indicated above with the
later methods taking higher precedence for a given section. However, the CollabHub only uses RENDERER section
resources; the other sections are ignored.
The ‘-chres file_name’ command line option specifies the pathname to a resource file. If multiple ‘-chres’
options are specified, only the last will be used.
The ENSIGHT9_RES environment variable specifies a resource file name that the CollabHub reads.
ENSIGHT9_RENDERER_HOSTS specifies a quoted string of space delimited host names (e.g. “host1 host2 host1
host3”) to be used for EnSight distributed renderers.
If the ‘-use_lsf_for_renderers‘ command line option is specified, then the CollabHub will evaluate the
environment variable LSB_MCPU_HOSTS for the resources. The environment variable specifies a quoted string such

Page 86

as “host1 5 host2 4 host3 1” which indicates 5 CPUs should be used on host1, 4 CPUs should be used on
host2, and 1 CPU should be used on host3. The hosts will be used in a round-robin fashion.
If the ‘-use_pbs_for_renderers’ command line option is specified, then the CollabHub will evaluate the
environment variable PBS_NODEFILE for the resources. The environment variable specifies a filename in which the
file contains list of line delimited host names that were allocated by the PBS scheduler.
The ‘-res file_name’ command line option specifies the pathname to a resource file. This command line option
can be specified multiple times. The last occurrence of a particular section takes precedence when multiple ‘-res’
options are given.
When using distributed rendering, any hosts specified via a prdist file are used instead of those given by RENDERER
resources. Additionally, any prdist file specified directly to the collabhub, will override one specified to the client.

A Client/Server Example
Resources are not used to specify where a server runs when it is part of a normal client/server session. The default
server connection in the Connection Setting dialog determines on which computer the server runs unless the Client
command line option ‘-c connection_name’ is specified.

A Simple SOS Example
The SOS can read any of the supported file formats in addition to the SOS Case file format. When a SOS Case file is
not used, then the number of EnSight Servers used is equal to the number of hosts specified in the SERVER resource
section.
1. The following resource file ‘my_hosts.res’ is created:
#!CEIResourceFile 1.0
SOS:
host: borg
SERVER:
host: drone1
host: drone2
host: drone3
host: drone1
2. EnSight is started with this command line:
ensight92 -res my_hosts.res -sos
The EnSight Client will automatically check out a gold key and will run on the local workstation, the SOS
(ensight92.sos) will be automatically started on computer ‘borg’ and will connect back to the client. Borg will need to
recognize the name of the computer that the client is running on.
3. In the File->Open dialog the LS-Dyna file ‘d3plot’ is selected and the ‘Load All’ button is clicked.
The SOS will start four EnSight Servers on computers ‘drone1’, ‘drone2’, ‘drone3’, and ‘drone1’ (presumably,
‘drone1’ might be a SMP). The ‘drone’ computers need to recognize the hostname borg in order to connect back to
the sos running on this computer.
Each of the servers will read 1/4 of the data set since the ‘Auto Distribute’ flag (on the SOS tab of the File->Open
dialog) is on by default for the LS-Dyna reader.

Another SOS Example
1. EnSight is started with this command line:
ensight8
2. The Case->Connection Settings dialog is opened. On the ‘SOS’ tab, an entry for host ‘borg’ is created. For
that entry, ‘Executable:’ is set to the name of command file ‘my_sos’, ‘Use default rsh cmd’ is
deselected, and ‘Alt rsh cmd:’ is set to ‘ssh’. The entry is saved and EnSight is terminated.
3. The following resource file ‘my_hosts.res’ is created:

Page 87

#!CEIResourceFile 1.0
SOS:
host: borg
SERVER:
host: drone1
host: drone2
host: drone3
host: drone1
4. On computer borg (assuming it’s running Unix or Linux), the file ‘my_sos’ is created:
#!/bin/csh
setenv ENSIGHT9_SERVER_HOSTS ‘cat $PBS_NODEFILE‘
ensight92.sos $*
The file must be in the user’s default path and must be executable.
5. EnSight is started with this command line:
ensight92 -res my_hosts.res -sos
The EnSight Client will check out a gold license key and run on the local workstation, the command file ‘my_sos’
will run on computer ‘borg’ which must be able to connect back to the local workstation by hostname. The client will
start up ‘my_sos’ via ssh. ‘my_sos’ sets the environment variable ENSIGHT9_SERVER_HOSTS to be the contents
of the file specified by the environment variable PBS_NODEFILE (OpenPBS’ dynamic list of allocated nodes).
6. In the File->Open dialog the LS-Dyna file ‘d3plot’ is selected and the ‘Load All’ button is clicked.
The SOS will start EnSight Servers on computers specified in file $PBS_NODEFILE. Hosts specified in the SERVER
section of my_hosts.res are ignored since ENSIGHT9_SERVER_HOSTS takes precedence.
Each of the servers will read 1/N of the data set since the ‘Auto Distribute’ flag (on the SOS tab of the File>Open dialog) is on by default for the LS-Dyna reader.

A SOS Case File Example
When a SOS Case file is used with resources, it needs to be modified otherwise the resources will be ignored for the
EnSight Servers. This is done for backwards compatibility.
1. The file SOS case file ‘big_data.sos’ is modified. Two lines are added to the FORMAT section:
‘use_resources: on’ and ‘auto_distribute: on’. The ‘casefile: ‘ line for each server is brought to
the beginning of each subsection.
FORMAT type: master_server LS-DYNA3D
use_resources:
on
auto_distribute:
on
SERVERS
number of servers: 2
#Server 1
#--------casefile:
d3plot
machine id:
executable:
ensight92.server
directory:
/tmp
login id:
data_path:
/tmp
#Server 2
#--------casefile:
d3plot
machine id:
executable:
ensight92.server
directory:
/tmp
login id:
data_path:
/tmp
Page 88

Note that the ‘casefile:’ line must appear before the other lines for that server
when using resources.
2. The following resource file ‘my_hosts.res’ is created:
#!CEIResourceFile 1.0
SOS:
host: borg
SERVER:
host: drone1
host: drone2
host: drone3
host: drone1
2. EnSight is started with this command line:
ensight92 -res my_hosts.res -sos
The EnSight Client will run on the local workstation, the SOS (ensight92.sos) will run on computer ‘borg’.
3. In the File->Open dialog the SOS Case file ‘big_data.sos’ is selected and the ‘Load All’ button is clicked.
The SOS will start two EnSight Servers on computers ‘drone1’ and ‘drone2’. Only two servers are used since two
‘casefile: ‘ lines occur in the SOS Case file. The ‘number of servers: 2’ line is ignored as are the
‘machine id:’ lines.
Each of the servers will read half of the data set due to the line ‘auto_distribute: on’ in ‘big_data.sos’.

Another SOS Case File Example
1. The file SOS case file ‘big_data.sos’ is modified. Two lines are added to the FORMAT section:
‘use_resources: on’ and ‘auto_distribute: on’. The ‘number of servers:’ line is modified. One
server subsection is specified.
FORMAT
type: master_server LS-DYNA3D
use_resources:
on
auto_distribute: on
SERVERS
number of servers:
#Server 1
#--------casefile:
machine id:
executable:
directory:
login id:
data_path:

4 repeat

d3plot
ensight92.server
/tmp
/tmp

2. The following resource file ‘my_hosts.res’ is created:
#!CEIResourceFile 1.0
SOS:
host: borg
SERVER:
host: drone1
host: drone2
host: drone3
host: drone1
2. EnSight is started with this command line:

Page 89

ensight92 -res my_hosts.res -sos
The EnSight Client will run on the local workstation, the SOS (ensight92.sos) will run on computer ‘borg’.
3. In the File->Open dialog the SOS Case file ‘big_data.sos’ is selected and the ‘Load All’ button is clicked.
The SOS will start four EnSight Servers on computers ‘drone1’, ‘drone2’, ‘drone3’, and ‘drone1’. Since the
‘number of servers:’ line has the word ‘repeat’, the servers specified in the SERVERS resource is used to
determine the number of servers used and their host names. All server subsections after the first in
‘big_data.sos’ are ignored due to ‘number of servers: 4 repeat’.
Each of the servers will read 1/4 of the data set since the ‘Auto Distribute’ flag (on the SOS tab of the File>Open dialog) is on by default for the LS-Dyna reader.

A PRDIST Example
1. The following resource file ‘my_hosts.res’ is created:
#!CEIResourceFile 1.0
SOS:
host: borg
SERVER:
host: drone1
host: drone2
host: drone3
host: drone1
COLLABHUB:
host: curly
RENDERER:
prologue: “xhost +”
host: larry
host: moe
2. The following prdist resource file ‘my_conf_with_res.prdist’ is also created:
#ParallelRender EnSight 1.0
router
pc
client
3. EnSight is started with this command line:
ensight92 -res my_hosts.res -prdist my_config_with_res.prdist
The EnSight Client will run on the local workstation, the SOS (ensight92.sos) will run on computer ‘borg’.
The EnSight CollabHub will run on computer ‘curly’. Two distributed renderers will start on hosts ‘larry’ and
‘moe’.
The my_conf_with_res.prdist file here specifies both "router" and "client" followed by blank names which indicate to
use the 'my_hosts.res' file. The "pc" option indicates to use parallel compositing which removes the GUI from the
composited display
NOTE: if "pc" is not specified, then a GUI will wrap the composited display - which is a testing and debug mode. In
addition, no display sync will be used during interactive transformations, producing a lag effect which is quite
annoying.
4. In the File->Open dialog the LS-Dyna file ‘d3plot’ is selected and the ‘Load All’ button is clicked.
The SOS will start four EnSight Servers on computers ‘drone1’, ‘drone2’, ‘drone3’, and ‘drone1’ (presumably,
‘drone1’ might be a SMP).
Each of the servers will read 1/4 of the data set since the ‘Auto Distribute’ flag (on the SOS tab of the File>Open dialog) is on by default for the LS-Dyna reader.

Page 90

Note that a prdist file can be specified as an option to the ‘-prdist’ command line option. However, if the defaults
are adequate or overridden with command line options, then a prdist file is no longer needed. Furthermore, specifying
the command line option ‘-prdist’ automatically implies the command line option ‘-sos’; previous versions
required the user to specify it. See “Distributed Memory Parallel Rendering” on page 18. of the User Manual for prdist
file documentation, including default values and manual connect support.

OTHER NOTES
See “Resource File Format” on page 13. in Chapter 10 of the User Manual for details on the resource file syntax.
See the EnSight User’s Guide for details on relevant SOS Case file modifications as they pertain to resources. Also,
see that section regarding details on which file formats support auto distribution. Note that not all Case files (i.e. nongold) can be auto distributed.
The default SOS and server entries in the Connections Setting dialog will be used as the template for SOS and
server computers not specifically listed in the dialog. This is useful for specifying defaults such as to use ‘ssh’ in place
of ‘rsh’ or to specify a default path.

SEE ALSO
How To Read Data
How To Read User Defined
How To Setup for Parallel Computation
User Manual: Server-of-Server Casefile Format
Resource File Format
Shared-memory parallel rendering
Distributed Memory Parallel Rendering

Page 91

Save or Output
Save or Restore an Archive

INTRODUCTION
EnSight command files are useful for restoring the system to a state reached in a previous session. However,
restoring a long session dealing with large files can be a tedious process. Fortunately, EnSight provides an archiving
mechanism that saves only the current state of the system, rather than the entire history of a session.
This capability is useful not only for large data files with several active variables, but also for saving a standard
starting point for sessions. In the initial session, geometry can be loaded, variables activated, a good viewpoint
selected, and an archive written. Subsequent sessions take advantage of this investment by merely loading the
archive (which can be done as you start EnSight from the command line).
The client and server each write separate binary files containing the complete current state of the respective
processes. Since these files are binary, they can be quickly written and restored. Note that an archive only contains
information resident in either client or server memory at the time of the archive. No information is available for
variables that were inactive or time steps other than the current. For this reason, you should never remove the
original dataset and attempt to use the archive as a substitute (unless you know what you’re doing).

BASIC OPERATION
An EnSight archive consists of three files:
1. The Archive Information File. This file provides pointers to the client and server archive files as well as additional
information required to load the archive. An example is given in the Advanced Usage section below.
2. The Client Archive file. This is the client’s binary dump file.
3. The Server Archive file. This is the server’s binary dump file.
(Note that for Server-of Servers, there will be an SOS archive file and then a server archive file per server)
Although each file has a default location, you can override the default during the archiving process.

Saving an Archive
1. Close all open EnSight windows except the main window.
2. Select File > Save > Full Backup... to open the Save Full Backup Archive dialog.

2. If desired, enter a new name for the Archive Information file. You can set the directory for
the Archive Information File by clicking the Archive Information File... button to open a
standard File Selection dialog.
3. If desired, select a directory for the client’s binary dump file by either entering the directory
in the Client Directory field or clicking the Client Directory... button to open a standard File
Selection dialog.
4. If desired, select a directory for the server’s binary dump file by either entering the
directory in the Server Directory field or clicking the Server Directory... button to open a
standard File Selection dialog.
5. Click Okay.

Page 92

You also have the option of saving an archive as you exit EnSight.
1. Select File > Quit... to open the Quit Confirmation
dialog.
2. Click the “Save full backup archive to:” toggle,
and either enter a new name for the Archive
information file or browse to the desired location/
file by clicking the Browse: button.

3. If you browsed to the file, click Save once
you have selected or entered the desired
filename.
This will place the filename in the Quit
confirmation dialog.

3. Click Yes to save the archive and exit.

Restoring an Archive
You can restore an archive either as part of EnSight startup or during an active session. To load an archive on
startup:

Page 93

1. Use the “-ar archive_info_file” option when you start EnSight. For example,
% ensight92 -ar load.ar
where load.ar is an Archive Information file saved in a previous session.
To restore an archive during an active session:
1. Select File > Restore > Full Backup... to open the File Selection dialog.
2. Select the desired Archive Information file and click Okay.
3. If the original connection (when the archive was saved) was manual, you will need to manually restart the
server.

ADVANCED USAGE
There are times when you may want to modify the contents of the Archive Information file. If you wish to use the
archive on a different machine or change the location of the binary dump files, you can simply edit the file with a text
editor. The following example shows the contents:
Date saved
Path to client’s binary file
comment
Case internal number
Case name
Connect type (auto or manual)
Server host machine
Server executable
Server data directory
Alternate server login ID
Path to server’s binary file

Wed Apr 2 15:31:51 1997
client ./ensight0402_153151.clientbkup
# server for Case ‘Case 1’. **Warning Don’t Modify The Internal Number**.
case_internal_number 0
case_name Case 1
case_connect_type auto
case_connect_machine indigo2
case_connect_executable /usr/local/bin/ensight/server/ensight.server
case_connect_directory /usr/people/joe/data
case_connect_login_id
server ./ensight_c1_0402_153151.serverbkup

Note that there will be a section for all the case_ variables for each current case in the EnSight session. See How
To Load Multiple Datasets for more information on cases.

OTHER NOTES
Important note! Archives are typically not upwardly compatible with new major – and some minor – releases of
EnSight. For this reason, the complete current command file is also saved as part of the client’s binary dump. If you
attempt to restore an archive and EnSight determines that the archive is not compatible with the current release, the
command file will be restored to a default location.

SEE ALSO
User Manual: Saving and Restoring a Full backup

Page 94

Record and Play Command Files

INTRODUCTION
Most powerful software systems have a built-in language that provides additional levels of power and functionality to
complement and enhance a graphical user interface. EnSight is no exception. Any action that you can perform with
the mouse or keyboard has a counterpart in the EnSight command language. A sequence of commands can be
saved during a session to automate repetitive or tedious tasks. Command files can be automatically executed on
EnSight startup to initialize the system to a desired state. Execution of command files can also be bound to keyboard
keys for user-defined macros.

BASIC OPERATION
During an EnSight session, all actions are recorded and saved to a file known as the default command file. This file
name typically starts with “ensight_” and is saved in /usr/tmp on UNIX systems or C:\Documents and
Settings\\Local Settings\temp on Windows systems (unless you have redefined your TMPDIR environment
variable). The default command file can be saved (and renamed) when exiting EnSight.

Recording Commands
To record a series of commands:
1. Select File > Command... to open
the Command dialog.

2. Toggle the Record button on.

3. A File Selection dialog opens.
Select or enter the desired file to
save commands to and click
Save.
4. When you wish to stop recording,
toggle the Record button off.
Note: As long as the record filename
stays the same, the record button may
be toggled on and off at any time,
appending more commands to the file.
When a new record file is selected,
any existing commands in that file will
be overwritten.

Page 95

Playing a Command File
To replay a command file:
1. Select File > Command... to open
the Command dialog.
2. Click on the Browse button for load
field.
3. A File Selection dialog opens.
Select the desired command file
and click Open.
The command file will be loaded and the
commands to be executed will be shown
in black below the green current line
indicator in the History window.
4. Toggle the Play button on.
As commands are executed, they will be
shown in gray above the current line.
You can control command execution by
pressing the VCR style buttons to:
stop,
start,
and single step playback.
Once playback is stopped, you can use
the “Skip” button to skip commands.
Playback speed can be controlled using
the “Speed” slider.

Playing a Command File on Startup
You can execute a command file as part of EnSight startup using the “-p command_file” option when you start
EnSight. For example,
% ensight92 -p redo.enc
where redo.enc is a command file saved in a previous session.

Page 96

ADVANCED USAGE
Command files are simple ASCII text and can be edited with any text editor. To easily determine the command for a
given action, open the Command dialog and watch the list above the current line as you perform various operations.
Keep in mind that the successful execution of some commands depends on the proper state existing at the time of
execution. For example, creating a part when the parent part (as referenced by the part number) does not exist will
cause an error.
Command files can be nested: if you have a file that performs a certain task, you can “call” that command file from
another file with the “play: filename” command. When a play: command is executed, the command file being
played will be expanded in the History window, in a different color below the current line. Check the "Expand playfiles"
box to expand all played files ahead of time. When played files are nested, their commands will be shown in red,
yellow, green, blue and black respectively.
An “exit:” command will cause EnSight to quit. An “interrupt:” command will cause the command file to pause
execution and open the command dialog.
You can save the command file for the current session when you exit EnSight, or you can use File > Save >
Command from this session... to save the commands up to that point
Command language can be used to generate macros. See How To Define and Use Macros.
In addition to command files and macros, you also access the python interface through this dialog. This is explained
in detail in the Interface Manual. (see Chapter 6, EnSight Python Interpreter)

OTHER NOTES
Command files provide an excellent method of documenting problems or potential bugs encountered during your use
of EnSight. The command file can be transmitted to CEI electronically to help determine the nature of the problem.

SEE ALSO
How To Define and Use Macros
User Manual: Command Files
Interface Manual: EnSight Python Interpreter

Page 97

Print/Save an Image

INTRODUCTION
The image displayed in the Graphics Window can be saved to disk or printed in a variety of formats: JPEG, TIFF,
RGB (SGI), XPM, PNG and PPM are all formats that store single images in each file. The formats: Apple QuickTime,
EnVideo, MPEG1, MPEG2, MPEG4, AVI, Macromedia Flash Video, Macromedia Flash and Animated GIF all
support video streams. The PostScript format supports images, "move-draw" graphics and EPSF. The POVRAY
format saves the geometry of the scene in a form that can be read by the POVRAY off-line rendering package.
See below for Saving Animations

BASIC OPERATION
Basic Still Image Operation
1. Select File > Print/Save Image....
2. Select Set Format... to choose the desired
output format and format options.
(See Changing the Save File Format below)

3. Set the base filename to save the image to
disk.
The Prefix select... option will allow a standard file
save dialog to be used to fill in this field.

4. Set various options:
The 'Convert to Default Print Color' option will invert
the color of the display. For example, the background
can be changed from black to white.
The 'Show Plotters Only' option will print only the
plots in the display.

5. Select any advanced options.
The 'Advanced' tab brings up the following options:
Window size: The 'Normal' option picks a window the
same size as the current window. 'Full' picks a full
screen window. Other options select various NTSC and
DVD standards. The 'User defined' option allows the
user to select any size output image. Note: there are no
limits to the size of the image that can be rendered.
Some formats cannot handle extremely large images.
EnSight may need to render the scene in multiple
passes to render at larger sizes, which can slow
rendering down.
Render to offscreen buffer: EnSight can use off-screen
OpenGL 'p-buffers' on graphics cards that support them.
This avoids artifacts that can show up with on-screen
rendering.
Save multiple images: This option causes EnSight to save MTM files based on detached displays.
Number of passes: sets the amount of multi-pass anti-aliasing to use: higher is better quality.
Stereo: The current scene can be rendered in stereo, even if the target system is not capable of displaying it.
'Current' is the default and picks stereo or mono display, depending on the current display mode. Mono and
Interleaved select mono or traditional dual-image stereo. The remaining options allow for the saving of anaglyph
stereo images (seen through red/cyan or other glasses).
Screen tiling: if these are set to values other than 1, the image will be saved as an MTM file. The numbers specify
the number of tiles in X and Y that the saved image will be subdivided into.

6. Select OK (or Print) to save and/or print the image.

Page 98

Saving Animations
The current animation or flipbook can be saved to
disk by following these steps:
1) Use the record button
Save animation dialog

to bring up the

2) Select the format of the file to save
(See Changing the Save File Format below)
3) Set the base filename for the image.
The 'Prefix select…' option will allow a standard
file save dialog to be used to fill this field in.
4) Set the number of frames of the animation to
save
5) For various types of animations (flipbooks,
solution times and animated traces), select if
these will be animated during the saving
operation and if they should be reset to their
initial values before beginning the save
operation.
6) Select any advanced options.
The 'Advanced' tab brings up the following
options. These are described in detail in the Image
file saving section.
7) Selecting 'Ok' will begin recording the
animation.
Progress is displayed in the information text in the
main window. The recording can be aborted by
pressing the 'A' key while it is progressing.
For more information, see EnSight’s keyframe animation and Flipbook animation facilities.

Changing the Save File Format
This dialog is presented to the user when any of the 'Set
Format...' buttons are clicked. It allows for a specific file
format and saving options to be selected. The subsequent
image/animation saving operations will utilize this format. The
basic dialog is shown here, with a scrolling list of available
formats listed. The options specific to the selected format are
displayed on the right side of the dialog. Pressing the 'Ok'
button selects the new format, while 'Cancel' will close the
dialog without changing the format or any of its settings.
The file formats are actually provided via plug-in modules known
as UDILs. It is possible for users to provide their own formats, but
the options for ones shipped with EnSight are documented here.

Common options
There are a number of common options used by many (but not all) of the formats. These are at the top of the dialog on
the right and include:
· Color/Black and White: Selects between RGB and Grayscale output
· Saturation Factor: Set the saturation factor for color images. Full saturation is 1.0, no saturation (i.e. white) is 0.0.

· Framerate: Most animation formats allow for the rate of the frames (in frames per second, fps) to be set for the
animation to be recorded. Generally, the default is 30fps.

Page 99

Options for PostScript Format

The PostScript format handles primitives either as precise drawing instructions (e.g. move to here, draw a line to
here, fill this region) or as sampled images (pixel data). There are advantages and disadvantages to both.
Move/draw output is resolution-independent and will reproduce fine lines and text. Since even low resolution printers
have 3-4 times the resolution of a typical graphics workstation (in dots/inch), move/draw PostScript typically produces
higher quality output. However, for very large models, the output files can become quite large (even with visibility
culling on) and subsequent printing can be slow.
In contrast, image or pixel PostScript saves the pixels of the image in the Graphics Window. Such an image is, by
definition, fixed resolution. When printed, the pixels will be scaled to fit the page. Since the printer resolution is higher
than the screen resolution, each pixel must be printed larger than it appeared on the screen resulting in visible pixels
and jagged edges. To improve the quality of image PostScript output, EnSight will print only 3D geometry as pixels the remaining objects (annotation text, color legends, and plots) will be output as move-draw instructions and will
overlay the image.
Options exist for the generation of EPS format Postscript as well as the embedding of a Window preview image (for
import into PC Windows applications ONLY - see Other Notes below).
Element visibility can be used to reduce the number of primitives in the Postscript output.
The subdivision option can be used to subdivide geometry for smooth color and shading output.
Portrait or Landscape output orientation may be selected.
The page can be scaled by an arbitrary page scale factor.

Options for POVRAY Geometry Format
There are no options for the POVRAY file format.

Options for AVI Format
Note: AVI files are a Microsoft standard format for movies, audio, icons, and other data types and are based on the
'RIFF' core file format.
The options for this format are a little different for Unix and 32bit Windows. For Unix and Windows 64, the only
Compression options are 'MJPEG', 'RAW' and 'MPEG4'. The only other option is the ability to set the maximum
bitrate for the MJPEG4 compression scheme. On Win32, the system installed AVI codecs will be listed as
compression options, along with options to specify the rate of keyframing, a general quality factor (0-100) and the
desired bit-rate in kilobits/second.

Page 100

Uncompressed AVI files can be quite large for even small animations. You can compress these files on your Windows
PC using the EnVe 2.0 utility. It is capable of reading an AVI file (or any other animation file written by EnSight) and
translating it to another format, including recompressing any AVI files.
The AVI file format can have problems porting from platform to platform as the compression schemes are not always
supported on all platforms. The MJPEG scheme is fairly well supported (Windows users need to install the latest
DirectX runtime for it) and the RAW format has size limitation for 640x480 on some platforms. In general, the Indeo
Video formats (e.g. IV41) and cvid are fairly portable and can be played by Apple's QuickTime player as well.

Options for Windows BMP Format
There are no special options (other than the Common options) for this format.

Options for EnVideo Format
This format has the advantage of being one of the few that natively supports stereo image streams. It also has a
number lossless compression options and is recommended by CEI for archival/original animation output. EVO files
can be converted to any other supported format using the EnVe 2.0 tool without loss of quality. This cannot be said for
other formats.

There are four compression options:
Raw - lossless, no compression, very large files.
RLE - lossless, run-length encoded imagery.
GZ - lossless, uses the 'zlib' compression scheme, good balance for machines with faster processors.
JPEG - lossy compression that uses the 'quality' option (0-100). Best compression ratio, but sacrifices some
quality.

Options for Animated GIF Format
This format is intended for simple, low-quality output for Web pages. Most browsers will automatically playback .gif
animations without the need of any plug-in modules. The format is limited to 256color images, so the quality of the
images is poor, especially for smooth shaded images. The compression ratio can be quite high.

Options include:
Number of times to loop: sets the number of times the animation should loop before stopping
Interlaced video: optimizes for slow web connection incremental display
Transparent values: The R,G,B values (0-255) of a pixel color that should be set to "transparent" in the image.
For example, setting these to (0,0,0) will cause all black pixels in the animation to be made
transparent on playback. -1 values select that no pixel is transparent.
Page 101

Options for JPEG Format
This is a very portable, but lossy compressed format. The only option is a notional "Quality" setting that controls the
compression rate (0-100).

Options for MPEG1 / MPEG2 / MPEG4 Format
MPEG is a very portable standard for animations. MPEG1 files are the most portable. MPEG2 is essentially the basis
of DVDs and requires the licensing of a player codec to play them back (although most DVD players include the
necessary, licensed codecs. MPEG4 is the basis of formats like QuickTime and WMV. It is not yet a very portable
format, but it provides much better quality than MPEG1 or MPEG2 for the same bandwidth.

Two options exist for MPEG. The specific sub-type of MPEG (1/2/4) can be selected as well as a target bitrate in
kilobits per second.

Options for PNG Format
The PNG format is a lossless image format supported by many platforms and most web browsers.

The only option is the method for compression that trades off computational complexity for overall compression rates.

Page 102

Options for PPM Format
The PPM format is a common lossless Unix image format that includes full color pixmaps (PPM), grayscale images
(PGM) and bitmaps (PBM)..

The options allow for the selection of Binary or ASCII forms of these files.

Options for Apple Quicktime Format
This is a popular animation format on the Apple Macintosh computers and Windows systems. The player can be
downloaded as part of the iTunes package from www.quicktime.com. EnSight does not support all the codecs that
QuickTime does, only the MPEG4-based compression..

The bitrate option selects the target stream rate in kilobits per second. There is a compression method option, but the
only possible value at this time is MPEG4.

Options for SGI RGB Format
There are no special options (other than the Common options) for this format.

Options for LLNL SM Format
This format was developed by Lawrence Livermore National Labs specifically for support of large, tiled displays with
dynamic pan/zoom playback. Players for the format include xmovie and blockbuster (blockbuster.sourceforge.net).
The format is internally tiled and includes multiple resolutions of the animation in the same file..

Page 103

Options include:
Compression: Raw, GZ, JPEG and RLE Similar to the CEI EVO format
Quality: JPEG quality setting
Tilesize: the size of the edge of one tile. 256 uses 256x256 tiles, while 0 specifies no tiling
Resolutions: the number of lower resolution movies to include. If the original animation is 640x480 and the
number of resolutions is 2, the file will contain animations at: 640x480, 320x240 and 160x120.

Options for TIFF Format
Tiff is a very portable, lossless image file format.

The format has one option and that is the compression method. All the supported methods are lossless.

Options for XPM Format
This format is popular on Unix platforms and is generally used for icons, but can be used for any image.

The transparent options allow for the specification of R,G,B values (0-255) of a pixel color that should be set to
"transparent" in the image. For example, setting these to (0,0,0) will cause all black pixels in the image to be made
transparent. -1 values select that no pixel is transparent.

ADVANCED USAGE
There are also some excellent public domain (i.e. free) tools for manipulating images. ImageMagick is a public
domain, X-windows based program for displaying both images and animations (loaded as sequences of images) on a
wide variety of platforms. Visit the Web site
http://www.wizards.dupont.com/cristy/ImageMagick.html for more information.
One of the most popular, cross platform tools is the GIMP. This tool has nearly the full functionality of Photoshop and
can read/write all the image formats EnSight can. It is often installed by default on Linux platforms, but OSX, Windows
and other platforms are supported as well: www.gimp.org.

OTHER NOTES
Almost all desktop publishing, page-layout, or word-processing packages permit importation of Encapsulated
PostScript files. Macintosh packages recognize files by explicit file typing based on a four letter code (unlike UNIX,

Page 104

which has no intrinsic file-typing). This code is not stored in the file itself, but in an “information file” used by the Finder
(the Mac OS) to handle files. EPS files are recognized by the code “EPSF”. There are various methods of setting this
code. File transfer utilities such as “fetch” can set the code during the transfer process. The “FileTyper” utility can be
used to directly edit the Finder Information File. Unless this file type is set properly, it is likely that applications will
refuse to recognize your EPS. Send email to fetch@dartmouth.edu for information on fetch.
EPS files typically contain a “preview image” that lets the importing application display a facsimile of the actual
graphic for ease in interactive positioning, scaling, or clipping. There are different methods of specifying this image
(e.g. PICT resources for Macintosh or TIFF files for Windows). Unfortunately, the different methods of specifying the
preview image preclude EnSight from providing this capability for import into Macintosh applications. When you
import an EPS file, most Macintosh applications will display it as a gray box. You can, however, still resize and
position the image and it should print fine. EnSight can, however, attach a preview image that can be used by
Windows applications. Enable the “Windows (PC) Preview Capable” toggle in the Image Format Options dialog. The
suffix “.EPS” should be used for the resulting files.
Do not attempt to send a PostScript file containing a preview image to a printer!
Additional Notes:
1. The file is saved or printed from the EnSight client machine - not the server.
2. The printer command should not include the file name. For example, if you normally print with "lpr -Plaser1 file.ps"
then enter "lpr -Plaser1" in the To Printer Using Command field.
3. If you toggle on Convert to default print colors, all viewport background colors are changed to white and any object
(part, viewport border, annotation, etc.) currently colored pure white (RGB = 1,1,1) will be changed to black.
Resolution Control - Available in Print Dialog of Windows Version

Note the pulldown allowing resolution
to be increased. Increases here can
greatly improve the resulting printed
image, but will cause a slowdown in
printing time.

SEE ALSO
User Manual: Saving and Printing Graphic Images

Page 105

Save Geometric Entities

INTRODUCTION
EnSight has three internal writers that allow saving geometric data and variable values in Brick of Values, Case
(EnSight Gold) or VRML. EnSight also allows the user to create their own writer as a dynamic shared library that is
loaded at runtime and listed in the addition to the internal writer formats.

BASIC OPERATION
Saving Parts in EnSight Gold or VRML Formats
1. Select File >

2. Be sure the desired output format is selected.
3. Follow the instructions given.
4. Enter a file root name.
5. If the dataset is transient, specify the beginning, ending, and step values.
For EnSight Gold only:
6. Toggle to save as binary files or not.
7. If the dataset is transient you can choose to save the multiple timesteps in one file
(one file per variable). If you choose this option, you can also specify the maximum
file size.
8. Click Okay.
Both internal and user-defined writers have access only to the geometry of selected parts and each of their active
variables. For all writers except VRML, only parts located on the server can be saved. This includes all original
model parts, and the following created parts: 2D-clips, Elevated Surfaces, Developed Surfaces, and Isosurfaces.
The VRML internal writer saves all the visible parts on the client in their current visible state except for Parts which
have limit fringes set to transparent. The VRML file will be saved on the client.
Output in the EnSight formats is intended to provide a method to save both model and created parts (with active
variables) for subsequent reuse with EnSight. VRML output is intended for export to other systems.
Most World Wide Web browsers come with either built-in or plug-in support for VRML file viewing.
There are some important differences in how EnSight saves parts according to format chosen.
Case(EnSight Gold)

VRML

Which parts are saved?

All parts currently selected in the Main Parts List (except those indicated below) All visible parts

Saved from where?

EnSight server

EnSight client

Which parts cannot be saved? Any client-based part: contours, vector arrows, particle traces, profiles.

Page 106

Saving Parts in Brick of Values Format
1. Select File > Save > Geometric Entities...

2. Be sure Brick of Values is selected as the Format type.
3. Follow the instructions given.
4. Select the desired variable.
5. If the variable is a vector, select the component desired.
6. Select the sampling resolution.
7. Select the sampling format, Brick of Bytes or Brick of Floats.
8. Enter a file root name.
9. Click Okay.
Brick of Bytes and Brick of Floats is intended to give you an interface mechanism to volume rendering codes.
When you click the Okay button the selected parts are discritized to the resolution indicated using the box tool as the
bounds and orientation (x/y/z resolution refers to the x/y/z directions for the box tool).
For Brick of Bytes (BoB) format a value of 0 is reserved for undefined (i.e., the discritized point found no variable
information). The value of 1 is tied to all variable values less than or equal to the minimum palette value tied to the
variable chosen while 255 is tied to all values greater to or equal to the maximum palette value.
For Brick of Floats (BoF) format undefined values are assigned the undefined value indicated in dialog.
Both BoB and BoF files are written out without any metadata - only the values for the discritized points is written. The
order of the data is according to the following pseudo code:
num_values = 0
for(z=0; z Save > Geometric Entities...

2. Select the desired user defined writer format.
3. Follow the instructions given.
4. If the writer accepts parameters, enter any desired ones in the
Parameter(s) field.
5. Enter a file root name.
6. Save as binary or Ascii file, based on this toggle.
7. If the dataset is transient, specify the Time Step info.
(Note that some writers produce static data, and thus may only use the
Begin Time Step info)

8. Click Okay.
The userd-defined writers can call the routines of an EnSight API to retrieve, for example, nodal coordinates, node
ids, element ids of parts selected in the Parts window, to be passed by value to be used, manipulated and/or written
out in any format desired. The User-defined writer dialog includes a Parameter field that allows the passing of text
into the writer from the GUI. This text could contain extra options which the writer understands.
Several example writers (including source code header files, Makefile and the corresponding shared library) are
included to demonstrate this capability.
The Case (Gold) Lite reader is included to demonstrate how to exercise most of the API and output a subset of the
Case (Gold) format. Complex numbers and custom Gold format are not supported with this writer. The Case (Gold)
writer ignores the Parameter field. While the writer is not compiled, the source code of this writer, the required header
files, and the Makefile are included.
The Flatfile user-defined writer is designed to demonstrate the output of selected part nodal data (coordinates & IDs)
as well as active variable values (scalar and/or vector only) in a comma delimited format easily imported into other
applications. If any of the keywords ‘ANSYS’ or ‘force’ or ‘body’ is entered into the Parameter field, then Flatfile will
output an ANSYS body force file.
The STL user-defined writer is designed to write out the border geometry in the form of triangular 2D elements of the
selected part(s) at the beginning timestep. The end time and the step time are ignored. The STL format does not
support multiple parts in a single binary file, but does support multiple parts in a single ASCII file. Therefore, if multiple parts are selected and ascii is checked, the STL writer outputs an ascii file with the border of each of the parts. If
multiple parts are selected and binary is checked, the STL writer outputs a binary file containing a single border of the
multiple parts. The STL writer only saves the beginning timestep and ignores the End Timestep and Step By fields.
The STL writer ignores the Parameter field.

Page 108

There are some important differences in how EnSight saves parts according to format chosen.
User Defined Writers (UDW)
Which parts are available to the UDW?

All parts currently selected in the Main Parts List (except those indicated below)

Where are the available parts located?

EnSight server

Which parts are unavailable to the UDW? Any client-based part: contours, vector arrows, particle traces, profiles

More user-defined writers may be distributed with EnSight in the future.

ADVANCED USAGE
If Rigid Body Transformations Present
Since EnSight does something special with the model timeset when rigid body information is read (via the rigid_body
option in the casefile, or from a user-defined reader with rigid_body reading capability), you need to be aware of a few
important issues. EnSight assumes that the rigid body timeset encompasses the normal geometry timeset, and it
replaces the normal geometry timeset with the rigid body timeset - thus the following occurs when using this option.
1. If any created parts are in the list to be saved, EnSight will save as true changing coordinates. Namely, a geometry
file containing the coordinates for each part will be saved at each time. Upon re-reading this model, you will be able to
duplicate all actions, but it will be done as a true changing coordinate model. In other words, the original rigid_body
file nature will not be duplicated.
2. If the original model had static geometry and rigid body file information - and you do not have any created parts in
the list to be saved - saving will preserve the single static geometry and rigid_body file nature of the model. However,
if the original model had changing geometry, or if variables have been activated - the number of geometry/variable
files saved will be according to the rigid body timeset. This timeset often has many more steps than the original
timesets - so be wise about the number of steps you write. It is often important to use the “Step by” option to control
this.
3. Because of the things mentioned in 1 and 2 above - if you want to use the save geometric entities option in EnSight
to “translate” a rigid body model from a different format into the EnSight format, you may want to consider the following process. First, read in the model without the rigid body transformations, activate the desired variables, and save
the model. Second, read in the model with the rigid body transformations, do not activate any variables, and save the
model (with a different name). Edit the Casefile of the first model to use the model: and rigid_body: lines of the
second casefile instead of the first casefile.

SEE ALSO
User Manual: Saving Geometric Entities
Readme file is $CEI_HOME/ensight92/src/writers/README

Page 109

Save/Restore Context

INTRODUCTION
EnSight context files can be used to duplicate the current EnSight state with the same or a different, but similar,
dataset. The context file works best if the dataset it is being applied to contains the same variable names and parts,
but can also be used when this is not the case.

BASIC OPERATION
An EnSight context consists of a set of files: the context file itself as well as associated palette, view, and keyframe
animation files. The names of the associated files will be that of the context file with a standard extension.

Saving a Context
1. Select File > Save > Context... to open the Save Current Context dialog.

2. Toggle Save Current Case Only or Save All Cases.
3. Enter a name for the Context File.
You can set the directory for the Context File by clicking the
Select File... button to open a standard File Selection dialog.
4. Click Okay.

Restoring a Context
Three options:
1) Start EnSight and restore a context as described below. This will recreate the parts of the original dataset
and restore them to their saved condition.
2) Start EnSight, read a new dataset, cancel the part loader without creating parts, and restore a context as
described below. This will create the parts of the new dataset (mapping as directed) and restore the
context of the original dataset.
3) Start EnSight, read a new dataset, create the desired parts, and restore a context as described below. This
will do the mapping (as directed) of parts and restore the context of the original dataset.
1. Select File > Restore >
Context...
2. Select the case to
restore the context to.
Note: If the context file
contains information for
multiple cases, ignores the
selection
3. Enter or select the
desired context file
4. Click Okay.

Page 110

OTHER NOTES
The same part names (and variable names) do not have to exist in the new case. If this situation arises, a pop-up
dialog will appear where you will be asked to match the part names (or variable names) from the context file with the
parts (or variables) from the new case. This dialog is not available in batch mode. Therefore, you can’t use a context
file that needs matching in batch mode. If the number of parts between the two datasets match, then no mapping of
parts occurs and the parts will end up renamed to match the original case.
When restoring context files with multiple cases, the needed cases will be started, if needed, according to the
connection scheme of the current run of EnSight.
Flipbook animations are not restored using the context file because it is unknown at the time the context file is
created what state existed when the flipbook was saved.
If data is not read before restoring the context file, the data that was used when the context file was saved will be
loaded.
Context files use EnSight’s command language and other state files (such as palette, view, and keyframe animation)
to recreate the parts, variables, and view state.

SEE ALSO
User Manual: File Menu Functions

Page 111

Save Scenario

INTRODUCTION
Scenario files are used by CEI’s viewer products which are capable of viewing all geometry (such as parts,
annotation, plots, etc.) that EnSight can display, including flipbook, keyframe, and particle trace animations.
A “scenario” defines all visible entities you wish to view with EnLiten or Reveal and includes any saved views and
notes that you want to make available to the viewer user.

BASIC OPERATION
1. Create the display you want to share with
the EnLiten or Reveal user.
2. Select File > Save > Scenario...
to open the Save Scenario
dialog.
3. Select Single File to save a
scenario file only, or Project to
save the scenario, jpg image
file, and EnSight context file.
4. Choose the EnLiten (.els) or
Reveal (.csf) format.
5. Enter a name for the Scenario
file/directory.
Click the Browse... button to
open a standard File Selection
dialog.
6. Select whether all, visible or
selected parts will be included.
7. Select the Time/Animation
Options tab
and select the flipbook,
keyframe, transient and/or
particle trace animations.
Available options depends on
output format chosen under the
File tab.
8. Save the scenario.

Page 112

ADVANCED USAGE
After the scenario has been saved, you may add additional views, as well as notes.
9. To Save additional views, click the Views
tab.
10. Manipulate the view as desired.
11. Name the view.
12. Click Save current view button.
You can repeat steps 10 through 12 as desired.

13. To save notes, click the Notes tab.

14. Enter a subject for the note.

15. Type in the text of the note.

16. Click Save note button.
You can repeat steps 14 through 16 as desired.

Page 113

17. If the Format is Reveal, variables can be
saved in the scenario file, under the
Variables tab.

18. Select the output architecture for the
PackNGo scenario file. Note that this list
reflects which platforms of Reveal you have
installed on the computer currently running
EnSight.
19. Click 'Save packed scenario
executable...' to be presented with the Save
As dialog, where you can specify the name
of the PackNGo file that will be created.

OTHER NOTES
EnLiten and Reveal are geometry viewers only. As such they are not capable of creating or modifying any new/
existing information such as variables or parts, or of changing timesteps (EnLiten only).
Since EnLiten is only a geometry viewer, only keyframe transformation information is stored when saving a scenario
file, i.e., no transient data keyframing is possible (consider loading a flipbook instead).
PackNGo simplifies distribution of scenario files for other users as these files do not require that the other user have
Reveal installed on their computer. The PackNGo file is an executable that encapsulates Reveal for a user specified
computer platform (e.g. MS Windows, Linux 2.6) along with the specified Scenario file. A user can simply execute
this file on their computer and it will automatically run Reveal with the embedded scenario file. Reveal is not installed
on the user's computer. Note that a particular PackNGo file can only support a single computer platform whereas the
scenario file can be distributed to any version of Reveal.

SEE ALSO
User Manual: File Menu Functions
Page 114

Save/Restore Session

INTRODUCTION
EnSight session file is a single file used to restore an EnSight state. When a session file is restored, the current
case(s) are deleted, and new case(s) from the session file are loaded and restored to the saved state.

BASIC OPERATION
Saving a Session
1. Select File > Save > Session... to open the Save Current Context dialog.

2. Toggle ‘Pack Data’ if you wish to include contents from listed
directories (including the data itself) in the session file (for
portability).
3. Click ‘Save’ button to open a file save browser and name
the session file (use .ens suffix) and click ‘Save’.

Restoring a Session
Three options:
1) The 'Welcome to EnSight' screen on startup displays your most recent Sessions. Just double click on the
desired session to load the data and restore it.
2) Mac and Windows users can double click any EnSight session file (ending in .ens) and the file will restore.
3) Any time during your EnSight session you can browse for a session file from the EnSight main menu as
follows: File > Restore > Session.... and just located the session file using the standard file access
window.

OTHER NOTES
If you already have data loaded and restore a session, EnSight will delete all the cases, start anew and then restore
the session.
If you are restoring a session file containing information for multiple cases, then all of the cases will be restored.
When restoring session files with multiple cases, the needed cases will be started, if needed, according to the
connection scheme of the current run of EnSight.
Flipbook animations are not restored using the session file because it is unknown at the time the session file is
created what state existed when the flipbook was saved.
All Session files are machine and operating system independent. However the data file(s) used in a non-packed
session file must remain in same directory in order to find the data file(s). In contrast, Packed Session files include all
the data files therefore can be moved to a different directory. The tradeoff is that Packed Session files can become
quite large.
Session files are machine and operating system independent. However the restoring platform must include all the
data readers necessary to read the data format(s) contained in the session.

SEE ALSO
User Manual: File Menu Functions

Page 115

Output for Povray

INTRODUCTION
EnSight can output a file which can be read into POVRAY (Persistence of Vision Ray Tracing). This allows EnSight
images to be able to have shadows and reflections which ray tracing can provide. POVRAY must be downloaded and
installed separately from EnSight (www.povray.org).
Note: This option requires that you have an EnSight Gold license and only works using nodal variable data.

BASIC OPERATION
The process is:
1. Run ensight and produce the desired image in the graphics window.
2. Go to File > Print/Save Image and set the Format to POVRAY Geometry and save.
This will produce the following files (samples of which are given in the Other Data section below):
filename.pov
filename.inc
ensight_to_pov_globals.inc
3. Edit ensight_to_pov_globals.inc as desired to control global information. You may also edit the filename.inc file
which contains information for each part.
4. Run POVRAY
povray width=800 height=600 filename.pov
This will produce the file:
filename.png
5. Run envideo92 using this file:
envideo92 filename.png

EnSight Images - No POVRAY

EnSight Images which have been run
through POVRAY

Page 116

OTHER DATA
ensight_to_pov_globals.inc
This is the editable text file to be used to customize the camera and lightsource information, and the part by part color
and material properties (ambient, diffuse, specular, roughness, and reflectivity). This file will be included into
filename.inc and parameters in this file will supersede the default values in filename.inc.
////////////////sample ensight_to_pov_globals.inc //////////////////////
//
// This file is useful in controlling multiple file outputs
// (i.e., output from the keyframe animator). Uncomment/edit items
// and they will be used instead of the settings in the .inc file
//
// Uncomment this next line if you uncomment anything
//#declare display_warning = 1;
//#declare camera_location = <-0 0 8366.19>;
//#declare camera_look_at = <-0 0 -16.7612>;
//#declare camera_angle
= 28.000000;
//#declare light_location
//#declare light_color

= <-15241.7 15241.7 76191.9>;
= rgb <1 1 1>;

// This will set reflective value for all parts
//#declare reflect_value
= .1;
// If you want to set the color for a part you would do this
// (useful if you have many .pov files since all the .inc files
// include this file)
//#declare Part_1_material = texture {
// pigment { color rgbt <1. 0. 0. 0.> }
// finish {
//
ambient 0.3
//
diffuse 1.0
//
specular 0.0
//
roughness 0.2
//#ifdef (reflect_value)
//
reflection reflect_value
//#else
//
reflection .1
//#end
// }
//}
#declare Part_495_material = texture {
pigment { color rgbt <0.600000 0.600000 0.600000 0.000000> }
finish {
ambient 0.300000
diffuse 1.0
specular 0.000000
roughness 0.027778
#ifdef (reflect_value)
reflection .2
#else
reflection .2
#end
}
}

Page 117

filename.inc
This text file has a statement that includes ensight_to_pov_globals.inc and then has the default global camera and
lightsource information as well as default Part by Part values of color and material properties.
///////////////////////sample filename.inc /////////////////////////////
#include “ensight_to_pov_globals.inc”
#ifdef
#debug
#debug
#debug
#debug
#debug
#end

(display_warning)
“\n*********************************************************\n”
“
\n”
“ Have applied settings for ensight_to_pov_globals.inc!!
\n”
“
\n”
“\n*********************************************************\n”

camera {
#ifdef (camera_location)
location camera_location
#else
location <-0 0 8837.74>
#end
#ifdef (camera_look_at)
look_at camera_look_at
#else
look_at <-0 0 0>
#end
#ifdef (camera_angle)
angle camera_angle
#else
angle 28.000000
#end
}
light_source {
#ifdef (light_location)
light_location
#else
<-14334 10667.6 78331>
#end
#ifdef (light_color)
color light_color
#else
color red 1 green 1 blue 1
#end }
#ifndef (Part_1_material)
#declare Part_1_material = texture {
pigment { color rgbt <1.000000 0.000000 0.000000 0.000000> }
finish {
ambient 0.300000
diffuse 1.0
specular 0.300000
roughness 0.027778
#ifdef (reflect_value)
reflection reflect_value
#else
reflection .1
#end
}
}
#end
#ifndef (Part_2_material)
#declare Part_2_material = texture {
pigment { color rgbt <1.000000 0.000000 0.000000 0.000000> }
finish {
ambient 0.300000
diffuse 1.0
specular 0.300000
roughness 0.027778
#ifdef (reflect_value)
reflection reflect_value

Page 118

#else
reflection .1
#end
}
}
#end

filename.pov
A text file that has a statement including filename.inc to define camera, lightsource and Part properties. The
remainder of the file contains coordinates and connectivity defining the surface of the Ensight parts as Povray surface
triangular elements. This file shouldn’t be edited by the user.
//////////////////////sample filename.pov ////////////////////////////
#version 3.5;
#include “carapov00.inc”
#declare Part_1=
mesh2 {
vertex_vectors {
297
<-243.353, -1002.62, 3.4535>,
<723.621, -213.728, -129.889>,
<731.815, -205.655, -144.313>,
<740.01, -197.583, -158.737>,
<748.204, -189.51, -173.161>,
<722.484, -203.276, -123.341>,
<730.534, -195.257, -137.655>,
<738.584, -187.239, -151.97>,
....
}
face_indices {
490,
<1,2,6>,
<1,6,5>,
<2,3,7>,
<2,7,6>,
<3,4,8>,
...
}
}
#declare Part_2=
mesh2 {
vertex_vectors {
2001
<-243.353, -1002.62, 3.4535>,
<788.215, -136.402, -241.148>,
<781.139, -143.803, -228.672>,
...
}
face_indices {
490,
<1,2,6>,
<1,6,5>,
<2,3,7>,
<2,7,6>,
<3,4,8>,
...
}
}
object {
Part_1
texture {Part_1_material}
scale <-1 1 1>
}
...
object {
Part_495
texture {Part_495_material}
scale <-1 1 1>
}

Page 119

Manipulate Viewing Parameters
Rotate, Zoom, Translate, Scale

INTRODUCTION
EnSight provides global transformations (rotation, translation, and zooming) to permit user manipulation of objects in
the Graphics Window. The transformations can either be performed interactively with the mouse, or precisely by
entering explicit values. The mouse buttons can be user-programmed to perform different transformations.

BASIC OPERATION
The Transformation Control Area controls the operation of the left mouse button (by default) in the Graphics Window.
The icon of the current action will be highlighted (e.g. Rotate is current below):
Selection Tool
Rubber-band Positioning

Rotate

Open the Reset Tools and
Viewport(s) dialog

Zoom

Translate

Open the Transformation
Editor dialog

Rubber-band zoom

Store / Recall
stored view

View from directions

Undo last transformation

Fit to window
Select Part [or View] mode in the Mode Selection area.
To rotate:
1. Click the rotate icon.
2. Move the mouse pointer into the Graphics Window.
3. Click and hold the left mouse button and:
• move the mouse left and right to rotate about the screen Y (vertical) axis, or
• move the mouse up and down to rotate about the screen X (horizontal) axis, or
• hold down the Control key and move the mouse left and right to rotate about the screen Z axis.
4. Press the F1, F2 or F3 keys for 45 degree rotation about the X, Y, or Z axis, respectively. Hold the Control
key down for -45 degree rotation. (Note: cursor must be in the EnSight window for F keys to work)
5. Press +X to view the scene from the positive X axis (looking toward the origin). The +Y, +Z, -X, -Y, -Z
buttons are similar. Press the “Last” button to get the scene back to the view that existed before any of
the +/-XYZ keys were pressed.
To translate:
1. Click the translate icon (or use the middle mouse button in steps 2 and 3 (default)).
2. Move the mouse pointer into the Graphics Window.
3. Click and hold the left mouse button and:
• move the mouse left and right to translate in the screen X (horizontal) direction, or
• move the mouse up and down to translate about the screen Y (vertical) direction, or
• hold down the Control key and move the mouse left and right to translate in the screen Z
direction.
To zoom:
1. Click the zoom icon (or use the middle mouse button in steps 2 through 5 (default)).
2. Move the mouse pointer into the Graphics Window.
3. Click and hold the left mouse button.
4. Drag down to zoom in or drag up to zoom out.
5. Hold down the Control key and move the mouse to pan.
To rubber-band zoom:
1. Click the rubber-band zoom icon.
2. Move the mouse pointer into the Graphics Window and position it at one corner of the desired viewing
region.
3. Click and hold the left mouse button.
4. Drag to include the desired viewing region. An outline of the region will appear as you drag.

Page 120

To rubber-band zoom using the selection tool:
1. Click the Selection Tool Rubber-band Positioning icon.
2. Move the mouse pointer into the Graphics Window and position it approximately at one corner of the
desired viewing region.
3. Click and hold the left mouse button.
4. Drag to include the desired viewing region. An outline of the region will appear as you drag.
5. Manipulate the tool as desired, by clicking at the center and dragging to a new position or clicking on any
corner and resizing. (Note that the aspect ratio will be preserved as indicated by the dotted lines within the
tool.)
6. Click the zoom (magnifying glass) indicator at the top left of the tool.
Note that zooming actually changes the location of EnSight’s virtual “camera” or “look-from” point. Zooming in moves
the camera closer to the object; zooming out moves it farther away. The look-from/look-at points can also be edited
explicitly.
If you have multiple viewports visible, each one can be manipulated independently. To transform in a different
viewport, place the mouse pointer within the bounds of that viewport before you click the left mouse button.
You can reset transformation parameters (as well as tool and frame transforms) by clicking the Reset.... See How
To Reset Tools and Viewports for more information.
The Fit button is useful in causing the currently visible parts to be centered and zoomed to fit within the viewport.

ADVANCED USAGE
All EnSight transformations can be controlled precisely by specifying explicit transforms in the Transformations Editor
dialog. To open the dialog, click the Transf Edit... icon on the desktop. The slider performs the requested
transformation (based on the selected transformation action) in the selected viewport(s).

Select the desired
transformation action.
Slider to specify
transform.
Set (by clicking within
the desired region) the
viewport that the
transform applies to.

To interactively perform
transformations on multiple
viewports, Control click on
multiple viewports, then
toggle on.

Specify axis to which
the transform applies

Increment controls the
step size for the slider
end arrows.
Enter explicit values in
the Increment field
(and press return) to
transform by a precise
amount.

Limit controls the sensitivity and
limit of the slider action.

You can also perform scaling in any or all dimensions (to, for example, magnify subtle differences in a surface).
Although you cannot perform the scaling operation with the mouse, you can scale using the Transformations dialog.
Click the Scale icon in the Transformation Control area and specify the scaling as described above.
You can copy the transformations from one viewport to another. First select the viewport you wish to copy, select
Editor Function->Copy Transformation State, then select the viewport(s) you wish to modify and select Editor
Function->Paste Transformation State.

Page 121

OTHER NOTES
By default, EnSight uses the left mouse button for performing the selected transformations. You can, however,
program the transformation action attached to each mouse button. See Customize Mouse Button Actions for more
information.
The transformation operations described here also apply to frame transformations. If additional frames have been
created and if the mode has been set to Frame, then any transform will apply to the currently selected frame. See
Create and Manipulate Frames for more information.
Pressing the F5, F6, or F7 keys while the mouse is within the EnSight graphics window or desktop area will transform
the scene to show a standard right, top, or front view, respectively. Pressing the F8 key will return the scene to that
which existed prior to F5, F6, or F7 being pressed. Further, holding the Control key down while pressing F5, F6, or F7
will store the current view to the selected Fx button.
Pressing F9 while the mouse is in the Graphics Window or the desktop area will zoom the display to full screen.
Press F9 again to return to the normal display.

SEE ALSO
Other viewing operations:
How To Set LookFrom/LookAt
How To Set Z Clipping
How To Create and Manipulate Frames
How To Reset Tools and Viewports
How To Use the Selection Tool
User Manual:
Global Transform
Frame Transform

Page 122

Set Drawing Mode (Line, Surface, Hidden Line)

INTRODUCTION
EnSight provides two basic drawing styles for graphics objects: line or shaded. Line mode draws only the line
segments of an object – regardless of the whether the lines are polygon edges or not. Shaded mode displays all
objects consisting of polygons (e.g. element or cell faces) as solid filled regions with light source shading enabled.
These drawing styles can be enhanced by enabling hidden-line mode. If the current mode is line, hidden-line will
eliminate all those lines that would be invisible if the object were a solid surface. If the current mode is shaded,
hidden-line mode will draw lines overlaying face edges. In shaded mode, hidden-line overlays are particularly useful
for visualizing computational grids.
The setting of line or shaded mode is a global toggle. You can also set the mode on a per part basis so that some
parts are displayed as lines and others as shaded surfaces. Each viewport also provides individual controls so that
the drawing mode can differ from viewport to viewport.

Line mode

Shaded mode

Hidden-line mode

Hidden-line overlay mode

BASIC OPERATION
The global toggles for shaded and hidden-line mode are available from the desktop. You can also enable these
modes by selected View > Shaded or View > Hidden Line. To use the desktop toggles:
1. Click the Shaded toggle to switch from line to
shaded mode (or vice-versa).
Line

Shaded

2. Click the Hidden Line toggle to enable or
disable hidden-line mode.
If the current mode is Shaded when you toggle on
Hidden Line, the Hidden Line Overlay dialog is
displayed. This dialog allows you to specify a color for
the overlay edges. If Specify Line Overlay Color is not
enabled, overlay color will be set to the native color of
each part. If it is enabled, the color can be specified
either by entering red, green, blue color values, or by
clicking the Mix... button and picking a color with the
standard Color Selector dialog.

Unhidden

Hidden

Page 123

The per-part toggles for shaded and hidden-line mode are available in Part mode.
1. Select Part in the Mode Selection area.
2. Click the Shaded toggle to switch from line to
shaded (or vice-versa).

Line

Shaded

3. Click the Hidden Line toggle to enable or
disable hidden-line mode.
Unhidden

Hidden

Note that enabling shaded mode for a part has no effect unless the global shading toggle is also enabled (on the
desktop or under the View menu). The same is true for hidden-line: unless the global hidden-line toggle is enabled,
the part will be drawn without hidden lines.

ADVANCED USAGE
Drawing modes can also be set on a per-viewport basis. As with per-part settings, these toggles require that the
corresponding global toggle is also set to have any effect.
1. Select VPort in the Mode Selection area.
2. Select (click in) the desired viewport in the Graphics
Window.
3. Click Viewport Special Attributes... to open the
Viewport Special Attributes dialog.
4. Click the Shaded button to disable shading in the
current viewport.
5. Click the Hidden Line button to disable hidden-line in
the current viewport.

OTHER NOTES
When a part is drawn in shaded mode (with or without hidden-line overlay) the surface is displayed with light source
shading enabled. EnSight uses two pre-defined light sources: one at the look-from point (the camera) and one on the
opposite side of the model (for back-lighting). The location of one of the light sources can be changed, see How To
Control Lighting Attributes.
In computer graphics, the appearance of a shaded surface is governed by a lighting model controlled by various
parameters. In EnSight, these parameters are part of the part’s attributes and can be changed on a per-part basis.
See How To Set Attributes for more information.

SEE ALSO
How To Control Lighting Attributes
User Manual: Global Shaded, Global Hidden Line

Page 124

Set Global Viewing Parameters

INTRODUCTION
EnSight provides various modes that control global viewing behavior. Three of these modes are discussed here:
perspective/orthographic projection, bounding box display modes, and static lighting.
EnSight can display viewports in either perspective or orthographic projection. A perspective projection is how we
normally view the world: objects that are farther away appear smaller. An orthographic projection removes this effect:
objects appear the same size regardless of distance. The projection setting can be specified on a per-viewport basis.
By default EnSight draws every point, line, and polygon for every visible part each time the Graphics Window
updates. For very large models (or slow graphics hardware), this behavior leads to unresponsive manipulations since
the update lags behind the corresponding mouse motion. Fortunately, EnSight provides other display modes that
improve responsiveness. Fast Display mode displays all visible parts in a reduced fashion during interactive
manipulation. This can be a bounding box representation, a point cloud representation, a reduced polygon
representation, an invisible representation, or if using immediate mode - a percentage of each part’s elements. When
the mouse button is released, parts are drawn normally. The Fast Display mode can also be set such that the
bounding display is used until the mode is changed - even when the mouse is released. (Edit->Preferences...
Performance - Static Fast Display)
Surface shading operations are expensive for very large models. Since the shading is dependent on the orientation
of the model with respect to the light sources, the surface colors must be recalculated each time the model moves.
Static lighting mode precalculates surface colors for a given orientation and then uses these colors during
subsequent transformations, resulting in improved interactive response.

BASIC OPERATION
Perspective/Orthographic Projection
The projection mode can be toggled either from a menu (View > Perspective) or in the VPort icon bar. To set the
projection from the icon bar:
1. Select VPort in the Mode Selection area.
2. Select (click in) the desired viewport in the Graphics
Window.
3. Click Viewport Special Attributes... to open the
Viewport Special Attributes dialog.
4. Click the Perspective button to toggle the projection
type in the current viewport.

Note that a viewport will only display a perspective projection
if the global toggle (as set with View > Perspective) is on as
well.

Page 125

Fast Display Mode
The Fast Display Mode can be set either from a menu (View > Fast Display > ) or by the Fast Display toggle on the
desktop. To change between the Dynamic or Static operation of this mode, go to Edit->Preferences... Performance.
To change the part representation for Fast Display Mode:
1. Click the Fast Display Representation pulldown icon.
2. Select Dynamic Box.
or
3. Select Points.
or
4. Select Reduced poly.
or
5. Select Invisible.

Note, if not using immediate mode, this
Sparse Model option will not be
available here.

Select Off to return to standard display
mode.

ADVANCED USAGE
If using immediate mode, and you desire to use the Sparse Model option for Fast Display, you can control the
percentage of the model that is displayed. See “Performance Preferences” . This mode is intended for large
models. It generally will not be pleasing (nor should it be needed) for small models.

SEE ALSO
User Manual: See “Part Mode”

Page 126

Set Z Clipping

INTRODUCTION
As you apply zoom transformations in EnSight, you may have noticed that the model begins to progressively
disappear as you move close to the model. This happens when the visible model parts intersect the front Z clipping
planes. The Z-clip planes (which are always perpendicular to your line of sight) are specified as distances from the
look-from point (the camera position). The Z clipping plane positions can be set by the user and can be used to
remove unneeded geometry from the display. Each viewport has it’s own set of Z clipping planes. By default, the Zclip planes adjust (float) with the model - thus stay out of the way if possible.

BASIC OPERATION
The initial position of the Z clipping planes is set based on the Z (depth) extent of the visible geometry – plus quite a
bit extra to leave room for transformations. The plane positions can only be set via the Transformation Editor dialog.
1. In the Transformation Control area, Click Transf... > Editor Function > Z_clip to open the
Transformation Editor.
If the Float Z-Clip Planes With Transform option is on,
The graphics display shows the relative positions
you can specify the minimum Z value that the Front clip
of the front and back clipping planes (left and right
plane can float to.
vertical red lines) to the Z extent of all currently
visible objects (white box).
2. Toggle the Float Z-Clip Planes option on to
have the Z-clip planes automatically adjust.
OR
Toggle the option off to manually adjust the
Z-clip plane locations.
If the Float Z-Clip option is off, you can edit the
plane positions either by dragging the red lines or
by entering explicit values in the Front and Back
text fields. Recall that the values represent the
distance from the look-from point to the plane.
3. Place the mouse pointer over the desired
plane marker and click the left mouse
button.
4. Drag the marker left or right to the desired
location. The Graphics Window will update
as the marker is moved.
– OR –
3. Enter explicit values in the Front and/or
Back text fields and press return.

If the markers become difficult to manipulate due
to changes, click the Redraw Z-Clip Area Above
button to rescale the markers.

Each viewport maintains it’s own independent Z clipping planes. The operation described above will change the
planes for the current viewport (as set by clicking in the desired viewport in the Graphics Window).
Note that clicking Reinitialize, in the Reset Tools and Viewport(s) dialog found under the Reset... button of the
Transformations area, will reset the Z clipping planes of the current viewport based on the Z extent of all objects
currently visible in that viewport.

OTHER NOTES
EnSight uses your workstation’s graphics hardware to implement Z clipping. The same hardware is used for Zbuffering – determining which objects are visible based on Z (depth) values. The Z buffer typically provides 24 bits of
resolution. EnSight attempts to make the best use of this limited resolution by setting the front and back clipping
planes reasonably close together. If the planes are too far apart, relative Z resolution is reduced and the hardware
Page 127

may not be able to accurately determine surface visibility. If you see artifacts like this, move the clipping planes
closer together.
EnSight also provides an additional clipping plane: the auxiliary clipping plane. Unlike the Z clipping planes which are
always perpendicular to your line of sight, the auxiliary clipping plane can be placed at any location in any orientation.
The Plane Tool specifies the location of the auxiliary clipping plane. By default, all geometry on the negative Z side of
the Plane Tool is removed. However, you can specify auxiliary clipping on a per part basis – some parts are clipped
while others are not. See How To Set Auxiliary Clipping for more information.

SEE ALSO
How To Define and Change Viewports, How To Set Auxiliary Clipping
User Manual: Z-Clip

Page 128

Set LookFrom / LookAt

INTRODUCTION
In addition to providing control over model manipulations, EnSight also provides control over the virtual camera used
to view the scene in the Graphics Window while in Global Transform Mode. If a viewport is being viewed through a
camera, this section is not applicable. The two control parameters are the look-from point (the position of the
camera) and the look-at point (a point on the camera’s line-of-sight vector). The Global Axis is positioned at the lookat point and is always in the center of the Graphics Window.
Initially, the look-at point is set to the geometric center of all visible objects and the look-from point is set to a point on
the positive Z axis such that all visible objects fit in the Graphics Window (as shown in the top image below). The
white axis triad is the Global Axis and can be displayed by selecting View > Axis Visibility > Axis - Global. The bottom
image shows the view after the look-from point has been repositioned between the X and Z axes. The diagrams to
the right of each image show a top-down schematic of each viewing case.
x

z

x

z

BASIC OPERATION
The look-from, look-at points are controlled via the Transformation Editor dialog.
1. Click Transf... in the Transformation Control Area.
2. Select Editor Function > Look At/Look From.

Page 129

Viewer Area for
interactive
manipulation

Viewer Area plane
toggles

Text fields for
entering numeric
values
Text field for
moving look-from
by setting an
explicit distance

The Transformation Editor dialog provides two methods for setting the look-at and look-from points. Numeric values
can be entered directly into the X,Y,Z Look At, Look From text fields (remember to press return). You can also enter
a value in the Distance field to explicitly move the look-from point a certain distance away from the look-at point.
Alternately, the Viewer Area can be used to interactively manipulate the points. The presentation of the Viewer Area
depends on the which plane toggle is set: X-Y (view from the positive Z axis), Y-Z (view from the positive X axis), or
X-Z (view from the positive Y axis – the default). In each case, the gray box represents the extent of all visible parts.
The intersection of the two red lines is the look-from point. The opposite end of the long red line is the look-at point
(which is initially near the center of the gray box). The example below shows the X-Z Plane presentation, the others
behave analogously.
To change the look-from point:
1. Place the mouse pointer over the
intersection of the two red lines.

To change the look-at point:
1. Place the mouse pointer over the free
end-point of the long red line.

2. Click and drag to the desired
location. Note that the Graphics
Window updates as the look-from
point is moved.

2. Click and drag to the desired location.
Note that the Graphics Window
updates as the look-from point is
moved.

During your manipulation, the display in the View Area may become difficult to use. Click the “Redraw Viewer Area
Above” button to rescale the display.
The Viewer Area Control Lock pull-down menu effects interactive operation in the Viewer Area as follows:
None

No constraints are placed on movement of either the look-from point or the look-at point.

Distance

Movement of the look-from (look-at) point is restricted to a circle whose radius is the current Distance
value and whose center is the look-at (look-from) point.

Together

The movement of both points is locked such that movements applied to one are applied to the other.

You can easily reset the look-from and look-at points such that all currently visible parts are displayed. Click Reset...
in the Transformation Control area to open the Reset Tools and Viewports dialog. Click the Reinitialize button to reset
the currently selected viewports.

Page 130

OTHER NOTES
You can also set the look-at point by picking an object with the mouse in the Graphics Window:
1. Click Reinitialize in the Reset Tools and Viewport(s)
dialog to clear all global transformations.
2. Click the Pick button in the global area above the
graphics window on the desktop.
3. Select Pick Look/At Point from the Pick Pull-down
icon.
4. Move the mouse into the Graphics Window. Place the
mouse pointer over the point you wish to set to the
look-at point and press the ‘p’ key (or whatever
mouse button you have set for “Selected Pick
Action” in Edit > Preferences > Mouse and
Keyboard).

Other camera parameters, such as the camera up direction and the field-of-view angle can be set in the dialog found
in the Transform Editor, Editor Function> Camera.

SEE ALSO
How To Define and Change Viewports.
How To View a Viewport Through a Camera
User Manual: Look At/Look From

Page 131

Set Auxiliary Clipping

INTRODUCTION
Unlike standard Z clipping where the front and back planes are always perpendicular to your line of sight, auxiliary
clipping lets you clip parts against a plane with arbitrary position and orientation. In addition, the auxiliary clip
attribute can be set on a per-part basis. This permits selective clipping to reveal objects of interest.
EnSight’s Plane Tool is used to provide the location for auxiliary clips. As the Plane Tool is manipulated (either
interactively with the mouse or via the Transformations dialog), the display in the Graphics Window updates to reflect
the new location of the plane.

BASIC OPERATION
Auxiliary clipping can be globally enabled by
selecting it in the View menu:

The Plane Tool will become visible and all objects on the negative Z side of the plane will be clipped (assuming the
plane currently intersects some visible part). You can now manipulate the Plane Tool to achieve the desired display
effect (see How To Use the Plane Tool for details). Note that Auxiliary Clipping always uses the infinite extent of the
plane specified by the Plane Tool – there is no way to restrict it to the rectangular bounds of the tool.
Each part has an attribute that controls whether it is clipped by the Auxiliary Clipping plane or not. To toggle this
setting:
1. Select the desired part (see How To Select Parts).
2. Select Part Mode in the Mode Selection area.
3. Click the Auxiliary Clipping toggle.
(This attribute can also be toggled in the Feature Detail Editor
dialog for the part. See How to Set Attributes for more
information.)

Off

On

SEE ALSO
How To Use the Plane Tool, How To Set Z Clipping.
User Manual: Part Auxiliary Clipping, Global Auxiliary Clipping

Page 132

Define and Change Viewports

INTRODUCTION
EnSight provides up to sixteen user-defined viewports in the Graphics Window. Each viewport is a rectangular region
of the screen (with or without a border) displaying some or all of the currently visible parts. Each viewport can be
transformed (e.g. rotated or zoomed), sized, and positioned independently. Viewports have several display
attributes including background and border color. Viewports provide a very flexible environment for data display.
This article is divided into the following sections:
Create a New Viewport
Select Viewports
Move and Resize Viewports
Set Viewport Background Color or Image
Set Viewport Attributes
Display Selected Parts in Viewports
Set Case Visibility Per Viewport
Perform Transformations in Viewports
Reset Viewport Transformations
Delete Viewports

BASIC OPERATION
Create a New Viewport
On startup, EnSight creates a single viewport that fills the Graphics Window. To create a new viewport:
1. Click VPort in the Mode Selection area to
enter Viewport mode.
2. Click the Viewports Layout pull-down icon
to select any of the standard viewport
layouts.
OR
2. Click the New Viewport icon.

Select Viewports
When you create a new viewport, it automatically becomes the currently selected viewport (as shown by the border
drawn in the default highlight color). Any action to change viewport attributes always operates on the currently
selected viewport(s). To select viewports:
1. Click VPort in the Mode Selection area to enter Viewport mode.
2. Move the mouse pointer into the Graphics Window and click the left mouse button anywhere within
the desired viewport. You can add to an existing selection by holding down the Control key as you
click in additional viewports.
To select all viewports, click the icon:

Note that the selected viewport is also changed in other modes (such as View) any time you perform some action
in a viewport (such as rotation). There is however, no visual feedback of this change until you enter VPort mode
again.

Page 133

Move and Resize Viewports
Viewports can be easily moved and resized. You can either reposition a viewport with the mouse in the Graphics
Window, or precisely by entering exact values. To move or resize a viewport:
1. Click VPort in the Mode Selection area to enter Viewport mode.
2. Select the desired viewport.
3. To move a viewport, move the mouse pointer into the Graphics Window and into the selected viewport.
Click and hold the left mouse button and drag the viewport to the desired location.
4. To resize a viewport, move the mouse pointer into the Graphics Window and place it over one corner of
the selected viewport. Click and hold the left mouse button and drag the corner to the desired
location.
To precisely reposition a viewport:
3. Click the Viewport Location Attributes icon
to open the Viewport Location Attributes
dialog.

4. Enter new values in the Origin X,Y, Width, or
Height fields (and press return).
The origin (at 0,0) is the lower left corner of the
Graphics Window. Note that the values are
normalized to the width and height of the default
viewport (i.e. the Graphics Window).
EnSight permits overlapping viewports. You can
control the ordering (from front to back):
Click The Viewport Forward icon to bring the
selected viewports to the top.
Click The Viewport Back icon to send the
selected viewports to the bottom.
Note: Viewport 0 is always displayed first, thus it
cannot be pushed or popped with these icons.

Page 134

Set Viewport Background Color or Image
Viewport background colors can be constant, blended, or inherited from the default viewport. To set viewport
background color:
1. Click VPort in the Mode Selection area to enter
Viewport mode.
2. Select the desired viewport(s).
3. Click the Color icon to open the Viewport
Background Color Attributes dialog.
The Type pull-down controls the type of background
coloring used. There are four types: Constant, blended,
inherit, and image.
Constant
A constant color will be used for the entire background.
To set a constant color:
4. Select Constant from the Type pull-down.
5. Either enter values in the RGB color fields (and
press return OR click the Mix Color... button to
open the Color Selector dialog.

6. Click Refresh Viewport.

Page 135

Blended
Up to 5 horizontal level colors can be specified with
interpolation between levels. To set a blended
background:
1. Select Blended from the Type pull-down.

2. Enter the desired number of levels in the # of
Levels field (and press return). Up to five
levels are supported.
3. To edit a color, first select it by clicking on the
number label in the Viewport Color window.
As shown, level 2 is currently selected.
Alternately, you can enter a value in the Edit
Level field or click the up/down arrows.
4. Change the selected color by either entering
new values in the RGB fields (and pressing
return) or clicking the Mix Color... button to
open the Color Selector dialog.
5. You can also change the relative vertical
position of a level by either clicking on the
level number with the left mouse button and
dragging up or down OR by entering a new
value in the Position field (and pressing
return).
6. Click Refresh Viewport.
Inherit
The selected viewports inherit the background type
and color from the default viewport. To set an
inherited background:
1. Select Inherit from the Type pull-down.
2. Click Refresh Viewport.
Image
The image specified will be used as the background
for the selected viewports. To set an image
background:
1. Select Image from the Type pull-down.
2. Enter the filename for the background image
to use or click the Select... button and
navigate to it.
Note, that the image must be either a .xpm or
.bmp file.
2. Click Refresh Viewport.

Page 136

Set Viewport Attributes
Viewports can be displayed with a variety of attributes:
1. Click VPort in the Mode Selection area to enter
Viewport mode.
2. Select the desired viewport(s).
3. Set the desired attribute as described below:
Click the Viewport Visibility Toggle to toggle display
of the selected viewports on or off (when not in
VPort Mode).

Off

On

Click the Viewport Border Attributes icon to open the
Viewport Border Attributes dialog.

Click the Visible toggle to display a border.
Enter values in the RGB fields (and press return) or
click the Mix... button to open a Color Selector
dialog.

Click the Viewport Special Attributes icon to open
the Viewport Special Attributes dialog.
Each viewport has it’s own toggles for perspective,
hidden surface, and hidden line drawing styles. These
controls will toggle the respective attribute for the
selected viewports. See How To Set Drawing Style
and/or How To Set Global Viewing for more
information.
In addition, a viewport can be 3D or 2D in nature. If the
viewport is designated as 2D, only planar parts may be
displayed in the viewport and transformations will
become 2D limited.
A viewport can be set such that it will track a node
number, a part centroid, or one of the part min or max
values. Thus as a model changes in time, the viewport
will stay centered on that location. See How To Do
Viewport Tracking for more information.

Page 137

Display Selected Parts in Viewports
Part visibility can be a set on a per-viewport basis such that some parts are visible in some viewports but not in
others. To set part visibility per viewport:
1. Select the desired part(s) in the Main Parts list.
2. Click the Part Visibility in Viewport Toggle icon.
The Part Visible in Which Viewport? dialog displays a
schematic of the current viewports. The part is currently
visible in the green viewports but invisible in the black
viewports.
3. Click in a green viewport to disable display of the
selected part(s) in that viewport OR click in a black
viewport to enable display of the selected part(s)
in that viewport.
Note that a similar interface for setting this attribute
appears in the General Attributes section of the Feature
Detail Editor dialog.

Set Case Visibility Per Viewport
If you have multiple cases in your session of EnSight, you can set viewport visibility for all parts associated with a
case. This makes it easy to display one case per viewport. To set case visibility per viewport:
1. Select the desired case from the Case menu (Case > casename).
2. Select Case > Viewport Visibility to open the Case Visible in Which Viewport? dialog.
3. Click in a green viewport to disable display of the selected case in that viewport OR click in
a red viewport to enable display of the case in that viewport.

Perform Transformations in Viewports
You can transform objects in a user-created viewport as easily as in the default viewport (See How To Rotate, Zoom,
Translate, Scale for details). For precise viewport transformations, you can use the Transformations Editor on a per
viewport basis:
1. Click Transf... in the Transformations Control
area.
2. To perform precise transformations in a
viewport, click the desired viewport in the
Which Viewport(s) window and perform the
transformation.
To select more than one viewport,
simultaneously hold down the control key
and click on additional viewports.
Note that this action will change the currently
selected viewport(s).

Page 138

Reset Viewport Transformations
The transformations for one or more viewports can be reset at any time in the Reset Tools and Viewports dialog.

1. Click the Reset... button on the bottom of the desktop.
2. Select the viewport(s) on which the reset will act.

3. Click on the appropriate button to perform the reset
action desired.
You can reset the selected action only, all rotates translates
and scales at once, or do a complete reinitialization of the
viewport.

Setting/Changing Viewport Part Bounds
Part bounds can be displayed within a viewport. This is useful for understanding the size of the model domain.

1. To turn on part bounds globally, toggle the
Bounds button on.

Page 139

2. To modify, in Vport mode, any of the settings
for the bounds display, click the Select
Viewport(s) Part Bounds Attributes icon.

3. Select General or the XYZ axes tabs.

4. Modify any attributes desired.
Including the visibility toggle if you don’t desire to
see the bounds in the selected viewports.

Delete Viewports
A created viewport can be deleted at any time:
1. Click VPort in the Mode Selection area to
enter Viewport mode.
2. Select the desired viewport(s).
(Hold down the control key to select multiple viewports)

3. Click the Delete icon.

Other Notes
You can interactively transform multiple viewports simultaneously by selecting the viewports you want to link together
and turning on the Link Interactive Transforms toggle. Those viewports that are highlighted in green will now
transform together for any transformations performed in the Transformation dialog. Linking does not apply to
transformations performed by the mouse in the graphics window.
You can copy the transformations from one viewport to another. First select the viewport you wish to copy, then select
Editor Function->Copy Transformation State. Next select the viewport(s) you wish to modify and select
Editor Function->Paste Transformation State.
Page 140

Shortcut
In Part Mode, right click on the background inside a viewport. You can change the view in the viewport, change the
viewport layout, or change the background color without ever changing to Viewport Mode.

SEE ALSO
How To Rotate, Zoom, Translate, Scale, How To Control Lighting Attributes
User Manual: VPort Mode

Page 141

Control Lighting Attributes

INTRODUCTION
EnSight allows control over the location of the light source for each viewport. This location is specified in terms of
Azimuth and Elevation relative to the viewport or in what is called “absolute position” - which is relative to the model
coordinate system. A intensity of a second light source can also be set, but its position is always at the viewer’s
(camera’s) location.

BASIC OPERATION
To specify the available lighting attributes In EnSight:
1. Click Vport mode.
2. Select the viewport(s) for which you want to modify the
lighting attributes.
3. Click the Selected viewports lighting button.
Which will bring up the Viewport lighting attributes dialog.
4. Choose whether lighting will be relative to the viewport
(Relative) or relative to the model axis system (Absolute).
5. Manipulate the position of
Light 1 by typing in Azimuth
and Elevation or using the
sliders.
6. If desired, also modify the
intensity of Light 2 (which is
at the viewer’s location).
If you are in Relative position
mode, you can convert to
Absolute by clicking.
Note that one can easily set the
light(s) back to the default
settings.

The effect of using a Relative position, is that when the model is rotated - the light source
does not rotate - so lighting changes on the model.
The effect of using an Absolute position, is that when the model is rotated - the light source
rotates with the model - so lighting on the model does not change.

SEE ALSO
User Manual: Lighting Attributes

Page 142

Display Remotely

INTRODUCTION
EnSight does not support the running of the client on one machine and setting the system display environment back
to a different machine. Not all of the features of OpenGL are supported on all platforms in this mode which can
conflict with EnSight’s graphics. It is intended that you actually run the client from the console of the client
machine.
If you run the client on a remote machine and display back, you will see the following warning displayed on the
console machine:
-------------------------------------------------------------------------Warning: EnSight has detected indirect OpenGL rendering. This could be
caused by remote display using X11, by an incorrect setting of the DISPLAY
environment variable, or by a bad driver installation.
When running using indirect OpenGL, you will notice a performance degradation
and loss of some rendering features. If you are running over a network we
strongly recommend that you install EnSight directly on the client machine.
EnSight is a client/server application, and you can run the EnSight server
on your remote machine.
-------------------------------------------------------------------------One way is to run the client on your local machine with a manual connection:
ensight92.client -cm
(Linux)
ensight92_client -cm
(Windows)
and on the remote machine:
ensight92.server -c clienthostname
(Linux)
ensight92_server -c clienthostname
(Windows)
Another way is to run your client and to tell it to open a connection on a remote machine (default is ssh) as follows
ensight92.client -c remotehostname

(Linux)

ensight92_client -c remotehostname

(Windows)

Running one or multiple servers remotely incurs no cost as only the EnSight client requires a license key.
And, of course the various VR combinations of display are valid.

SEE ALSO
How To Use Server of Servers
How To Setup for Parallel Rendering

Page 143

Save and Restore Viewing Parameters

INTRODUCTION

EnSight’s viewports provide a great deal of flexibility in how objects are displayed in the Graphics Window. Given the
complicated transformations that can be performed, it is imperative that users be able to save and restore
accumulated viewport transforms.

BASIC OPERATION
View saving and restoring is accessed from the Transformations dialog.

Saving Viewing Parameters
Click Transf... in the Transformations
Control area to open the Transformations
dialog.
1. Select the viewports you want to save.
Click within a viewport to select it. Hold
down the control key as you click to
select additional viewports.
2. Select Save View... from the File menu.
Select a directory and enter a file name
in the file browser and click OK.

EnSight provides a maximum of 16 viewports: the main viewport (which you cannot change) and 15 additional
viewports. When EnSight saves one or more viewports, it also includes the viewport number (which is equal to the
creation order) as a tag. When you request that one or more viewports be restored, EnSight looks in the saved file
and searches for tag numbers corresponding to the currently selected viewports. If it finds a match, it restores that
viewport. If there is no match for a selected viewport, it is left unchanged.

Restoring Viewing Parameters
Click Transf... in the Transformations Control area to open the Transformations dialog.
1. Select the viewports you want to restore. As shown above, click within a viewport to select it. Hold down
the control key as you click to select additional viewports.
2. Select Restore View... from the File menu. Select a file name in the file browser and click OK.

What is Saved
Only global and local (frame) transformations are stored in a view parameters file. No information is stored for
viewport attributes, look-from/look-at points, or Z clipping.

Other Notes
By default, the F5, F6, or F7 buttons restore a standard right, top, or front view (respectively) of the selected viewport.
However, by holding down the Control key while pressing one of these keys, the current view will be saved to that
key. Subsequent pressing of that key will restore the saved view. Only Global transforms are saved / restored by
these operations, not Frame transforms.

SEE ALSO
How to Define and Change Viewports, How to Create and Manipulate Frames.
User Manual: Save/Restore View
Page 144

Create and Manipulate Frames

INTRODUCTION
By default, all parts are assigned to the same frame of reference. You can, however, create additional coordinate
frames and assign parts to them. These frames (and the parts assigned to them) can be manipulated (rotated,
translated, scaled) independently of other frames. Some examples of frame usage:
1. You wish to create a copy of a part and display a different variable on the copy. When you create the copy, a new
frame is automatically created and the copy is assigned to it. The new frame can be translated away from the
original to visualize both variables simultaneously.
2. You wish to create an animation of parts moving independently (e.g. for an exploding view or to “open” a closed
object with a “hinged door”). Each dynamic part is assigned to a new frame. During keyframe animation, the
frames are manipulated independently to achieve the desired motion.
3. You have a dataset with rotational periodicity but the symmetry axis is not aligned with a major axis. A new
frame is created and positioned such that one of it’s axes is aligned with the symmetry axis.
4. You have a dataset that makes correct positioning of EnSight tools difficult, e.g. a duct not aligned with a major
axis. Create a new frame and align one of the axes with the duct. Since tool positions are always specified with
respect to the current frame, you can now use the Transformation Editor to accurately position tools along the axis
of the duct.
In addition to position and orientation, frames have a number of display attributes such as visibility, line width, and
color. You can also specify the length of each axis separately and display a series of evenly spaced labels to use as
a 3D measuring tool.
Frames are a powerful but complex feature of EnSight. Understanding the basics of frames is essential for proper
use. This article is divided into the following sections:
Introduction
Create a New Frame
Select Frames
Assign Parts to Frames
Move and Rotate Frames
Reset Frame Transform
Set Frame Attributes
Determine What Frame a Part is Assigned To
Delete Frames

Page 145

BASIC OPERATION
Introduction
On startup, EnSight creates a default frame – frame 0 – located at 0,0,0 of the right-handed “world” or model
coordinate system and aligned with the X, Y, Z axes. All parts (model and newly created) are assigned to frame 0
initially. Frame 0 is special in that it cannot be repositioned or deleted.
Note: Frame mode is reserved for the expert user. By default, it is not enabled. To enable it, go to Edit>Preferences..., select General User Interface and toggle on Frame Mode Allowed.
Frames are selected either by clicking the frame axis triad (while in Frame mode) in the Graphics Window or by
selecting the frame in the “Which Frame” list of the Transformation Editor dialog. Any frame operation (such as
setting attributes) acts on the currently selected frames.
The EnSight positioning tools (Cursor, Line, Plane, and Quadric tools) are always positioned with respect to the
currently selected frame. If more than one frame is selected, frame 0 is the reference frame for tools. If you have tools
visible, you will notice them changing position as the selected frame is changed.
EnSight implements computational periodicity (such as rotational symmetry) as an attribute of frames. If a frame has
symmetry enabled, all parts assigned to the frame will be duplicated as specified by the particular type of symmetry.
All frame axis triads are visible when in Frame mode. The axis triad consists of three lines representing the X, Y, and
Z orientation vectors plus labels. Selected frames are colored with the default highlight color (typically green). If the
frame is visible (meaning it will be displayed in all modes) the frame axes are drawn with solid lines. Otherwise,
dashed lines are used.
EnSight does not support hierarchical frames: you cannot assign a frame to another frame to implement nested
transformations. All frames are embedded in the same world coordinate system (i.e. frame 0).

Create a New Frame
In general, you have to explicitly create new frames. However, EnSight will automatically create a new frame each
time you create a copy of a part and assign the copy to the frame.
To create a frame:
1. Click Frame in the Mode Selection area to enter Frame mode.
(Note: If Frame does not appear as an available mode, first go to Edit>Preferences..., select General User Interface and toggle on Frame
Mode Allowed.)

The initial position of a new frame can either be set to 0,0,0 or
automatically centered on a set of parts.
2. If desired, select one or more parts in the Main Parts list – the new
frame will be centered on the selected parts.
3. Click the New Frame icon to create the frame.
The new frame also becomes the currently selected frame.

Page 146

Select Frames
There are two ways to select frames. You can click on the frame axis triad in the Graphics Window or select frames
in the “Which Frame” list in the Transformation Editor dialog. Selected frames are colored with the default highlight
color (typically green).
To select frames in the Graphics Window:
1. Click Frame in the Mode Selection area to enter Frame mode.
(Note: If Frame does not appear as an available mode, first go to Edit->Preferences..., select General User
Interface and toggle on Frame Mode Allowed.)

2. Position the mouse pointer over the frame axis triad (the lines – not the XYZ labels) and click the left
mouse button.
You can extend a selection of frames by holding down the Control key as you click on frames.
You can select all frames by clicking:

To select frames using the Transformation Editor dialog:
1. Click the Transf... icon in the Transformation
Control area to open the Transformation
Editor dialog.
2. Select Frame > Transform from the Editor
Function menu. Note that this puts EnSight
into Frame mode.
3. Select the desired frames in the Which Frame
list.
You can use standard Motif list selection techniques,
such as shift-click to extend a selection or controlclick to de-select an item.
The Which Frame list is also displayed if the Editor
Function menu is set to one of the Tool modes (e.g.
Tools > Cursor).

Assign Parts to Frames
To assign a part to a frame:
1. Click Frame in the Mode Selection area to enter Frame mode.
(Note: If Frame does not appear as an available mode, first go to Edit>Preferences..., select General User Interface and toggle on Frame
Mode Allowed.)

2. Select the desired part(s) in the Main Parts list.
3. Select the desired frame (as described above).
4. Click the Part Assignment icon to assign the part(s) to the frame.
A message is printed to the Status History area confirming the assignment.

Page 147

Move and Rotate Frames
You transform a frame (and all parts assigned to it) when you perform any transformation while in Frame Transform
mode. Frame Transform mode is set automatically when you enter Frame Mode. You can also set it explicitly from
the Editor Function menu in the Transformation Editor dialog.
To transform in Frame Transform mode:
1. Click Frame in the Mode Selection area to enter Frame
mode.
(Note: If Frame does not appear as an available mode, first go to
Edit->Preferences..., select General User Interface and toggle
on Frame Mode Allowed.)

2. Toggle the Transform/Definition button to be.
3. Select the desired frame(s) (as described above).
4. Perform the desired transformation either interactively
(using the Transformations Control icons and the mouse
in the Graphics Window) or via the Transformation Editor
dialog. See How To Rotate, Zoom, Translate, and Scale
for more information.

Frame transforms are implemented as a transformation applied with respect to the frame’s position and orientation.
At times you will need to modify the position and orientation of the frame independent of the parts assigned to it. This
is done while in Frame Definition mode. You enter Frame Definition mode either explicitly from the mode menu in the
Transformation Editor dialog (Editor Function > Frame > Definition), or via the Transform/Definition pull-down icon
while in Frame Mode.
Important! You cannot change the frame definition if you have performed any frame transformations (if you attempt
to do so, a dialog will remind you). Any frame definition must be applied prior to a frame transformation. If you have
already made frame transforms you can clear them by returning to frame transform mode and using the Reset Tools
and Viewports dialog (click Reset... to open).
To transform the Frame Definition:
1. Click Frame in the Mode Selection area to enter Frame
mode.
2. Toggle the Transform/Definition button to be.
3. Select the desired frame(s) (as described above).

4. Perform the desired transformation. This can be done either interactively (with the mouse in the
Graphics Window) or via the Transformation Editor dialog. To translate the frame interactively, move the
mouse pointer into the Graphics Window and click and drag the left mouse button. To rotate the frame
interactively, click and hold the left mouse button on one of the frame axes and drag the mouse. Clicking
on the X axis will rotate the frame about its Y axis. Clicking on the Y axis will rotate the frame about its X
axis. Clicking the Z axis will rotate about both X and Y. Use the Transformation Editor dialog to rotate
about the Z axis only.

Page 148

You can also edit the frame’s definition explicitly using the Transformation Editor dialog:
1. Click Frame in the Mode Selection area to enter Frame mode.
(Note: If Frame does not appear as an available mode, first go to Edit>Preferences..., select General User Interface and toggle on Frame
Mode Allowed.)

2. Click the Frame Location Attributes icon.
This opens the Transformation Editor dialog in Frame Definition mode.

3. Select the desired frame(s).

4. If desired, enter new value(s) in the XYZ
fields to change the frame’s origin
(remember to press return).
5. If desired, enter new value(s) for the
orientation vectors (remember to press
return).
Note that the orientation vectors are
normalized afresh when you press return.

Reset Frame Transform
The frame transform can be reset back to the default position and orientation by using the Reset Tools and Viewports
dialog. To clear the frame transform:
1. Click Frame in the Mode Selection area to enter Frame mode.
2. Make sure the Transform/Definition button is set to transform
3. Select the desired frame(s) (as described above).
4. Click the Reset... button in the Transformation Control area to open the
Reset Tools and Viewports dialog.
5. In the Reset Tools and Viewports dialog, click the desired button:
Reset By Selected Transform Only: clear only the transformation component
currently selected (e.g. rotate or translate) in the Transformation Control area
Reset Rotate/Translate/Scale: clear all transformation components
See How To Reset Tools and Viewports for more information.

Page 149

Set Frame Attributes
Frames can be displayed with a variety of attributes:
1. Click Frame in the Mode Selection area to enter Frame mode. (If needed, first enable Frame Mode
under Edit->Preferences..., General User Interface.)
2. Select the desired frame(s) (as described above).
3. Set the desired attribute as described below:
Click the Frame Visibility Toggle to toggle display of the axis triad of selected
frames on or off (when not in Frame Mode).
Off

On

Click (opens the Color Selector) to set the color for the axis triad of selected
frames.
Click the Frame Line Width pull-down to set the line width for the axis triad of
selected frames.
Click the Axis Triad Attributes icon to set axis attributes (described below).

To adjust the length of the frame axes, enter
new values in the X, Y, and Z Length fields and
press return.
To display a series of evenly spaced labels
along an axis (showing distance from the axis
origin), toggle on the applicable Label button,
enter the desired number of labels in the # of
field, and press return.

Page 150

Determine What Frame a Part is Assigned To
You can determine what frame a part is assigned to (and change it) by opening the Feature Detail Editor for the part:
1. Open the Feature Detail Editor for the
part type (Edit > Part Feature Detail
Editors >) or double click on the
appropriate Feature Icon.
2. Select the desired part in the parts list at
the top of the Feature Detail Editor.

3. Open the General Attributes section.
The part’s current frame number is shown in
the Ref. Frame field. You can reassign a part
to a different frame by entering a new value
and pressing return.

Delete Frames
Selected frames can be deleted. Note that a frame cannot be deleted if any parts are currently assigned to it. All
parts assigned to the frame must be assigned to other frames prior to deletion.
1. Click Frame in the Mode Selection area to
enter Frame mode.
2. Select the desired frame(s) (as described
above).
3. Click the Delete icon.

SEE ALSO
How To Set Symmetry, How To Rotate, Zoom, Translate, and Scale, How To Reset Tools and Viewports
User Manual: Frame Mode

Page 151

Reset Tools and Viewports

INTRODUCTION
EnSight provides support for complex transformations of various entities (e.g. the scene, tools, frames). It is often
necessary to clear all or part of the transformation associated with an entity; the Reset Tools and Viewports dialog
provides this capability.

BASIC OPERATION
To clear global transformations or tool positions:
1. Click Part in the Mode Selection area (to be sure
that EnSight is in Global Transform rather than
Frame transform).
2. Click the Reset... button in the
Transformation Control area to open the Reset
Tools and Viewports dialog.
3. Perform the desired operation as described
below.
4. Click Close.

Transformations will only be reset for
the current viewport(s). Click in a
viewport to select it. Control-click to
extend the selection or de-select a
selected item.

Click the applicable button to reset the
corresponding tool.

Toggle selects whether tool is
reset based on the global XYZ
space or reset based only on
the selected viewport.

Click to clear only the transformation
component currently selected in the
Transformation Control area (e.g.
Rotate or Translate).

Click to clear all transformations as well
as reset the camera look-from/look-at
points so that all currently visible parts
are centered in the selected viewport(s).
This also resets the center of transform
to the geometric center of the visible
parts.

Click to clear all
transformations in the
selected viewport(s). Note
that zoom is not a scene
transformation and is not
cleared. Zoom is
implemented by moving the
look-from point (the camera
position). To clear zoom, click
Reinitialize.

Page 152

ADVANCED USAGE
The Reset Tools and Viewports dialog is also used to clear Frame transformations. See How To Create and
Manipulate Frames for more information on frames and frame transforms.
To clear frame transformations:
1. Click Frame in the Mode Selection area to enter
Frame mode. (If needed, first enable Frame mode
under Edit->Preferences... General User Interface.)

2. Make sure the Transform/Definition button is in the
transform state
3. Select the desired frame(s).

4. Click the Reset... button in the Transformation
Control area to open the Reset Tools and
Viewports dialog.
5. Perform the desired operation as described
below.
6. Click Close.

Frame transformations will only be reset
for the current viewport(s). Click in a
viewport to select it. Control-click to
extend the selection or de-select a
selected item.

Click to clear only the frame
transformation component currently
selected in the Transformation Control
area (e.g. Rotate or Translate) for the
selected frame(s) in the selected
viewport(s).
Click to clear all frame
transformations for the
selected frame(s) in the
selected viewport(s).

SEE ALSO
How To Rotate, Zoom, Translate, Scale, How To Define and Change Viewports, How To Create and Manipulate
Frames

Page 153

Use the Color Selector

INTRODUCTION
Several operations in EnSight require that you select a color. The Color Selector dialog is used throughout the user
interface to provide a powerful and easy-to-use color selection mechanism.

BASIC OPERATION
The selector operates using one of two basic color models: RGB or HSV. The RGB color model specifies color by the
percentage of red, green, and blue and closely mimics the way computers deal with color. The HVS color model
specifies colors as percentages of hue (the actual color with red equal to both 0.0 and 1.0, green equal to 0.33, and
blue equal to 0.66), saturation (the “amount” of color, where 0.0 is white and 1.0 is full), and the value (the brightness,
where 0.0 is black and 1.0 is full). The HSV model is often more intuitive for mixing custom colors. Although HSV is
the default, you can switch to RGB by clicking the RGB toggle button.
The dialog provides four basic methods of selecting colors:
1. By picking one of the
predefined colors from the
grid of color cells.

Color square always displays
the current color selection.

2. By grabbing the marker in the
color cube and moving it with
the mouse.

4. By grabbing and moving the
sliders associated with each
color component.

3. By entering values for HSV
(or RGB, depending on
mode) directly in the fields
and pressing return.

When you have selected a color, click the Apply button to have the selected color applied to the object being edited
(e.g. part, color map level, text, etc.).

Specify Custom Colors
If you have colors that you use frequently that are not represented in the color grid, you can save them by replacing
selected cells. Your custom colors are automatically saved for future sessions. To set custom colors:
1. Select the desired color using any of the methods described above.
2. Toggle on Change Color Cell.
3. Click in the color cell you wish to replace.
4. Continue to select colors and replace cells.
5. Toggle off Change Color Cell when done.
The color information is saved in EnSight defaults directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older Windows, and ~/.ensight92 on Linux,
and in ~/Library/Application Support/EnSight92 on the Mac) with the following filename:
ensight.colpal.default.

SEE ALSO
User Manual: Color Selector

Page 154

Enable Stereo Viewing

INTRODUCTION
EnSight supports active stereo display on workstations with quad-buffered OpenGL stereo capability, in addition to
passive (polarized) stereo support for detached displays (see How To Setup Parallel Rendering). Active stereo
works by rapidly displaying alternating left and right eye views on the screen. An emitter (which sits on top of your
display monitor) sends an infrared signal to special glasses worn by the viewer(s). The glasses contain liquid crystal
shutters that alternately open and close the left and right eye lenses in response to the signal from the emitter in sync
with the monitor display. The update frequency is such that the viewer effectively fuses the left and right views into a
single stereo image.
Stereo is useful for viewing any type of visually complex geometry. It is especially helpful for visualizing amorphous
objects such as animating particle traces, trace ribbons, or discrete particles. It has also been noted that
management and customers are typically quite impressed by stereo display.

BASIC OPERATION
In EnSight, stereo display is enabled by pressing the F12 key on your keyboard. Pressing the F12 key again will
return to normal display. The stereo separation angle can be controlled by pressing the F10 and F11 keys. F10
decreases the angle and F11 increases the angle. When EnSight is configured to use a detached display (see How
To Setup Parallel Rendering), these commands affect only the detached display. The GUI window remains
monoscopic.

Configuring your display
On most platforms the display is not initialized by default in a mode which enables stereo viewing. In general quadbuffered stereo requires a refresh rate of 96Hz or higher. On some monitors it may be necessary to decrease the
display resolution in order to accommodate this higher refresh rate. Check your monitor documentation before
attempting to change the refresh rate.
There is a utility distributed with EnSight which can be used to determine if your display has stereo capability. Run
‘cei_apex21_glinfo’ from a command line and look for OpenGL visuals with a ‘y’ the column ‘st’ or ‘stro’. If none exist,
then the current display parameters do not allow for stereo viewing.
Below are example instructions for various platform configurations which have been tested and confirmed to work
with EnSight. When in doubt, refer to your system documentation for OpenGL as well as the X server (Unix) or video
adapter device driver (Windows).
Linux
Professional graphics cards generally support stereo OpenGL under Linux. Documentation is included with the
drivers, which may be downloaded from the card vendors web sites.
MS Windows
Configuration of stereo under Microsoft Windows is dependent upon the graphics card driver which is installed.
Right-click on the background and choose “Properties” to open to Display Properties dialog. Look for a tab which
such as “OpenGL Properties” or “Advanced” and search for a stereo option. In many cases there is a toggle button
for enabling stereo display. You will usually need to restart the machine in order for changes to take effect. If stereo
still does not work, try changing the display resolution, as stereo may not be available at higher resolutions.

Page 155

Pick Center of Transformation

INTRODUCTION
EnSight allows you to pick where you would like the center of transformation to be for the model.

BASIC OPERATION
1. Click the Pick button in the global area above the
graphics window on the desktop.

2. Toggle on Pick Center of Transformation.
3. Position the mouse cursor on your model at the
desired location for the center of transformation.
4. Press the “p-key” (or whatever mouse button you
have set for “Selected Pick Action” in Edit >
Preferences > Mouse and Keyboard).
Your model will now rotate about the position on the model
that you just picked.

You can also set or change the exact location of the center of transform by using the Transformation Editor.
1. Click the “Transf...” button on the desktop
below the graphics screen.
2. Under “Editor Function”, select “Center of
Transform”.
3. Set of modify the x,y,z coordinate location
of the center of transform in the dialog which
comes up.

Note: clicking on the ‘Fit’ button or the
‘Reset’ followed by the Reinitialize button will
reset the center of transform to the geometric
center of the visible parts.

SEE ALSO
User Manual: Center Of Transform

Page 156

Set Model Axis/Extent Bounds

INTRODUCTION
EnSight provides model axes and extent bounds to help in orienting your model. These features are toggled on/off via
the quick access area on the desktop.

BASIC OPERATION
Model Directional Triad
The model axes help maintain awareness of the principal directions of the reference frame of the model. This is
especially helpful during model transformations.

Click the Axis toggle to display the model directional
triad.

Page 157

Model Extent Bounds
The model extent bounds also help maintain dimensional information pertaining to the extents of the model.

Click the Bounds toggle to display the model extents

To control the various attributes associated with the model
extents:
1. Select the Viewport Mode icon.
2. Select the Model Extent Bounds icon, which opens the
Viewport 2D/3D Grid attributes dialog.
3. Modify the various general and/or axes attributes as
desired.

SEE ALSO
User Manual: Part Bounds Attributes

Page 158

Do Viewport Tracking

INTRODUCTION
EnSight provides the capability to “track” a particular location on the model parts displayed in a viewport. Tracking
means that the viewport will be caused to center on the chosen location as time is changed. This is particularly useful
for models with changing geometry or applied displacements - allowing one to stay focused on the moving bodies
during an animation.

BASIC OPERATION
Viewports can be displayed with a variety of attributes:
1. Click VPort in the Mode Selection area to
enter Viewport mode.
2. Select the desired viewport(s).
3. Click the Viewport Special Attributes icon to
open the Viewport Special Attributes dialog.

4. Select the Tracking option desired,
5. And supply the node or part id appropriately.
6. Change time step, load a transient flipbook,
or the like and note that the viewport will stay
centered on the location chosen.

SEE ALSO
How To Define and Change Viewports
User Manual: VPort Mode

Page 159

View a Viewport Through a Camera

INTRODUCTION
Global transform mode defines a viewing position and then allows you to transform (translate and rotate) the scene.
Camera mode behaves a little differently. In this mode the scene remains as defined and does not move. Instead the
scene is viewed through a camera which can be positioned at any location and oriented to look in a specific direction
and have a specified "tilt".
A viewport can either be in Global transform mode (default) or it can be defined to be viewed through the camera.
Local transforms are valid in either mode. In order to view a viewport through a camera (a) the camera position and
orientation must be defined, and (b) the viewport must be tied to a camera.

BASIC OPERATION
Any viewport can be viewed through a camera by
1. Click Transf... in the Transformation Control Area

2. In the resulting Transformation editor (Global
Transform) select the viewport you want to view
through a camera

3. Select the camera from the Tie viewport(s) to
camera pulldown. When set to None the camera
model is not used and the Global transformation
model is active.

If a viewport is being viewed through a camera the interactive transformations (when you click and drag the mouse
buttons in the viewport) affect the camera position and orientation. By default the visibility of the cameras are off.
There are eight total cameras available that can be manipulated. By default they are positioned at the +/- XYZ axis
locations plus two more cameras showing a view of -1 -1 -1 and 1 -1 -1.
To position/orient a camera interactively:
1. If you click-drag for a transform in a viewport being tracked by a camera the camera will transform
OR
1. In viewports that are not being viewed through a camera you will see a camera icon (if camera visibility is on). You
can click-drag the center of the camera to drag the camera to a new position. Clicking/dragging the axis of the
camera rotate the camera.
OR
1. You can set the Pick option from the Desktop area immedately above the graphics window to position/orient the
camera
2. Place the mouse pointer over the desired locaton on a part in any of the viewports in the graphics window and
press the 'p' key (or whatever mouse button you have set for the "Selected Pick Action" in Edit->Preferences->Mouse
and Keyboard). Depending on which pick action was chosen the camera will be positioned or oriented according to
the pick.
You may pick a spline control point for the Camera origin in which case the camera will position and orient itself
according to the spline.

Page 160

To turn on camera visibility:
1. Click Transf... in the Transformation Control Area
2. Select Editor function > Camera
3. Select the camera(s) you want to turn visible
4. Turn on the Visible toggle.
To position/orient a camera interactively from the
Camera Transformation editor
1. If the Origin is set to XYZ then the camera is located
at the X, Y, Z locations shown here
If the Origin is set to Spline then the camera origin
will be located on the defined spline
If the Origin is set to Node then the camera origin will
be located at a specified node id.
2. The camera orientation is controlled by the Camera
Z direction and the Camera Up vector. If the Focus is
set to Node or XYZ then the Z vector is defined by the
Node/XYZ location.
To set other camera attributes:
1. The view angle controls the field of view through the
camera. A small value simulates a telephoto lens
while a large value simulates a wide angle lens
2. The Size sets the size of the camera glyph. Use the
up/down arrows to increas/decrease the glyph size
by a factor of 2.

ADVANCED USAGE
1. If the camera origin is on a spline, zoom operations will move the camera along the spline
2. If the origin or Focus is set to a node number the camera will update if the node changes position.

SEE ALSO
How To Use the Spline Tool

Page 161

Manage Views

INTRODUCTION
EnSight provides a capability to save and restore viewing parameters for the data model and all viewports.
Collectively, this state is known as a View. This dialog portrays Views graphically as buttons with a small picture
("thumbnail") of the currently displayed data rendered with the underlying viewing parameters of that View.
With the Views Manager the user can create, save, restore, and apply viewing parameters in a simple point-and-click
interaction.

BASIC OPERATION
The Views Manager dialog is displayed by right clicking on
the EnSight graphics area background and choosing
View>Create New View
OR by selecting the 'Views…' button below the EnSight
graphics area
OR in the main menu Windows>Views Manager...
The dialog will look similar to that shown here.
(Initially, the Views Manager will not contain
any thumbnails of Views.)

Click on the ‘New’ Button (or right-click on an empty
area of the User Defined Views and select ‘New’) to
create a new view using the current orientation and
viewing parameters in the main graphics window.
The 'Save views' button will display a file browser in
which the user can select a directory. The manager
will then write each View into a separate EnSight
view file (named sequentially 'view0', 'view1',
'view2'...) A maximum of 16 Views can be used.
The button 'Restore views' will display a file
browser in which the user can select a directory to
scan for EnSight View files. Any Views found in that
directory will be loaded and displayed as a
thumbnail button with the currently loaded data.
Note that the 'Restore views' button will only look for
views created by EnSight 8.2.1(e) or newer. Older
Views must be loaded individually via the right-click
menu explained later.

Note: when restoring, the file browser has a toggle
button “Use stored images for thumbnails’ which when
set causes the originally stored image in the view to be
displayed on the thumbnail instead of the currently
loaded image. This can be useful if the current image
takes a long time to render.

Page 162

Clicking on a standard view will put the main
graphics window in that view. It does not create a
view in the User Defined Views.
Clicking a thumbnail button with the left mouse
button will apply that View to the EnSight graphics
window.
Clicking the
mouse's right
button will display
one of two pop-up
menus.
If the right mouse
button is clicked on
top of a thumbnail
image, then the
following menu will
be displayed.

Clicking the mouse’s right button in the
background of the
thumbnail drawing area
will display this menu.

The menu options perform the following actions:
Apply

Performs the same action as clicking the left mouse button on the selected thumbnail
button.

Add as keyframe (20)

Adds a keyframe with this view with 19 Sub-Frames.

Edit keyframe count

Pops up a window to query enter number of SubFrames, then adds a keyframe with this
view.

Replace

Replaces the thumbnail button's viewing parameters and image with the currently
displayed state of the EnSight graphics window.

Update image

Replaces the thumbnail button's image with the button's viewing parameters while using
the currently loaded data.

Delete

Deletes the selected thumbnail button and associated viewing parameters. Note that if
the View is associated with an EnSight View file, the file will not be deleted.

Save as...

Displays a file browser where the user can specify both a directory and an alternative
file name for the View.

New

Creates a new View button using the currently displayed model data and all viewports.

Update all images

Performs the same action as 'Update image' but for all thumbnail buttons.

Delete all

Performs the same action as 'Delete' but for all thumbnail buttons

Restore...

Displays a file browser where the user can select an EnSight View file to load. Note that
this option allows the user to load all versions of View files.

SEE ALSO
User Manual: Chapter 9: Transformation Dialog File Menu, Save/Restore View

Page 163

Manipulate Tools
Use the Cursor (Point) Tool

INTRODUCTION
EnSight provides a 3D point specification tool called the “Cursor” tool. When visible, the Cursor appears as a 3D
cross colored red (X axis), green (Y axis), and blue (Z axis). The Cursor tool is used to supply EnSight with point
information, for example to specify the location for a query or the starting point for a particle trace.

BASIC OPERATION
In many cases, the Cursor tool will automatically turn on when performing some function that requires it. You can also
turn the tool on and off manually by toggling the Cursor entry in the Tools menu or by clicking the Cursor toggle on the
Desktop.

The Cursor tool can be placed in three ways: interactively through direct manipulation with the mouse, by positioning
the mouse pointer over a part and pressing the ‘p’ key, or precisely positioned by typing coordinates into a dialog.
To position the Cursor with the mouse:
1. Place the mouse pointer over the center of the tool.
Note that the mouse cursor will change when over the center
of the cursor tool (if in Part or Frame mode).
2. Click (and hold) the left mouse button.
3. Drag the Cursor to the desired location.
4. Release the mouse button.
(Undo/Redo button at the bottom of screen can be used to undo/redo the
tool transformation)

Cursor translation is restricted to the plane perpendicular to your line of sight. If you need to move the cursor in
another plane, rotate the model such that the desired translation plane is perpendicular to your new line of sight.
(Note that the Cursor may not exactly track the location of the mouse pointer.)
To position the Cursor on a part with the ‘p’ key:
1. Click the Pick button in the global area above the
graphics window on the desktop.

2. Select “Pick cursor tool location” from the pop-up
menu.

3. Place the mouse pointer over the desired location on
a part in the graphics window and press the ‘p’ key
(or whatever mouse button you have set for the
“Selected Pick Action” in Edit > Preferences > Mouse
and Keyboard).

Page 164

To set the Cursor by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.
2. Select Editor Function > Tools > Cursor.

3. Enter the desired coordinates into the X, Y,
and Z type-ins and hit return.

You can also move the Cursor by setting the desired axis of translation in the Axis pop-up and manipulating the slider
bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit of the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Cursor since the X,Y,Z numeric
values always update to reflect the current location. If you are positioning the Cursor interactively with the mouse, the
values will update when the mouse button is released.

Shortcut
In Part Mode, right click on the cursor tool. You can hide the tool (make it invisible), edit it (open the Transformation
Editor), or use the tool to quickly do something such as query a variable over time, or emit a particle streamline trace.

ADVANCED USAGE
After a model has been loaded, the initial location of the Cursor is set to the “look-at” point – the geometric center of
all visible geometry. The coordinates of the Cursor are specified with respect to the default frame: frame 0. However,
if you have created additional frames, you can position the Cursor relative to the origin of a different frame. This is
accomplished by selecting the desired frame in the “Which Frame” list in the Transformation Editor dialog.
You can easily reset the position of the Cursor tool to the default. See How To Reset Tools and Viewports for more
information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Line, Plane, Box, Cylinder, Sphere, Cone, Surface of Revolution. See the How To article on Frames
for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 165

Use the Line Tool

INTRODUCTION
EnSight provides a 3D linear specification tool called the “Line” tool. When visible, the Line tool appears as a
(typically white) line with an axis system at the center point and an arrow head on one end. The Line tool is used to
supply EnSight with a linear specification, for example to specify the location for a line clip or a “rake” for a particle
trace.

BASIC OPERATION
In many cases, the Line tool will automatically turn on when performing some function that requires it. You can also
turn the tool on and off manually by toggling the Line entry in the Tools menu or by clicking the Line toggle on the
Desktop.

The Line tool can be placed or manipulated in three ways: interactively through direct manipulation of tool “hotpoints”
with the mouse, by positioning the mouse pointer over a part and typing the ‘p’ key, or precisely positioned by typing
coordinates into a dialog and/or rotating the tool about its axis. With surface normal options the line remains normal.
To move the Line with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Line to the desired location.
4. Release the mouse button.
To stretch the Line with the mouse:
1. Place the mouse pointer over one of the Line endpoints.
2. Click (and hold) the left mouse button.
3. Drag the endpoint to the desired location.
4. Release the mouse button.
To rotate the line with the mouse:
1. Place the mouse over the end of one of the tool axes.
2. Click (and hold) the left mouse button.
3. Drag the axis endpoint until the line has rotated as desired.
4. Release the mouse button.
Note selecting the X axis endpoint will rotate about the Y axis, selecting the Y axis endpoint will rotate about the X
axis, and selecting the Z axis endpoint will rotate in a general fashion about the centerpoint.
Note that the mouse pointer will change when it is over a hotpoint (if you are in Part or Frame mode).
(Undo/Redo button at the bottom of screen can be used to undo/redo the tool transformation)

Line moving and stretching is restricted to the plane perpendicular to your line of sight. If you need to move the Line
in another plane, rotate the model such that the desired translation plane is perpendicular to your new line of sight.
(Note that the Line will not exactly track the location of the mouse pointer.)

Page 166

To position the Line on a part with the ‘p’ key:
1. Click the Pick button in the global area above the
graphics window on the desktop.
2. Select “Pick line tool location” from the pop-up
menu. (Then pick either by 2 points or 2nodes.)

3. In the Graphics Window, place the mouse pointer on
a part over the desired location for the first Line
endpoint and press the ‘p’ key (or whatever mouse
button you have set for the “Selected Pick Action” in
Edit > Preferences > Mouse and Keyboard).
4. Move the mouse pointer to the desired location for
the second Line endpoint and again press the ‘p’
key.
When “Using 2 points” the endpoints will be place at the pick location.
When “Using 2 nodes”, the endpoints will be placed at the nearest
node and the ids of those nodes will be saved, such that the line tool
will continue to be attached to these nodes - even if they move.

To set the Line by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.
2. Select Editor Function > Tools > Line.

3. Enter the desired coordinates for the
endpoints into the X, Y, and Z fields and
press return.
3. Alternatively, you can enter the node ids for
two nodes in the model.
This has the effect of keeping the line tool tied
to the two nodes - even if they move over time.
Note the Length field - which is discussed in
Advanced Usage below.

Rotation, translation or scaling of the tool can also be accomplished by selecting the appropriate transform action
icon and the desired axis, and then manipulating the slider. In this case, the values in the “Scale Settings” section
control the sensitivity and limit of the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Line since the X,Y,Z numeric values
always update to reflect the current location. If you are positioning the Line interactively with the mouse, the values
will update when the mouse button is released.
Page 167

Shortcut
In Part Mode, right click on center selection point of the line tool. You can do quick x or y rotates, hide the tool, or
open the transformation editor. You can also use this right click to quickly create a line clip, query a variable, or do a
particle streamline trace with the line tool as the emitter.

ADVANCED USAGE
After a model has been loaded, the initial location of the Line center is set to the “look-at” point – the geometric center
of all visible geometry and parallel to the X axis. The coordinates of the Line are specified with respect to the default
frame: frame 0. However, if you have created additional frames, you can position the Line relative to the origin of a
different frame. This is accomplished by selecting the desired frame in the “Which Frame” list in the Transformation
Editor dialog.
You can easily reset the position and orientation of the Line tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.
To find the distance between two nodes that have IDs, you can use the calculator function Dist2Nodes. However, to
find the distance between two nodes on different parts, or between two nodes if one or both don’t have IDs, use the
line tool. Use the Pick Line Tool Location-> Using 2 nodes option as shown above, then move the cursor near the first
node location, hit ‘p’ key, move to the second node location and hit the ‘p’ key, then open up the transformation editor
and in the transformation editor menu, Edit>Tools>Line you’ll find the length of the line tool which is the distance
between those two points.

SEE ALSO
Other tools: Cursor, Plane, Box, Cylinder, Sphere, Cone, Surface of Revolution. See the How To article on
Frames for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 168

Use the Plane Tool

INTRODUCTION
EnSight provides a plane specification tool called the “Plane” tool. When visible, the Plane tool appears as a
(typically white) rectangular region with an axis located at the center point. The Plane can also have a semitransparent “filled” center that enhances visibility of the region. The Plane tool is used to supply EnSight with a
planar specification, for example to specify the location for a planar clip or a “net” for a particle trace.

BASIC OPERATION
In many cases, the Plane tool will automatically turn on when performing some function that requires it. You can also
turn the tool on and off manually by toggling one of the Plane entries in the Tools menu (e.g. Tools > Plane) or by
clicking the Plane toggle on the Desktop.

The Plane tool can be placed in three ways: interactively through direct manipulation of tool “hotpoints” with the
mouse, by positioning the mouse pointer over a part and typing the ‘p’ key, or precisely positioned by typing
coordinates into a dialog.
To move the Plane with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Plane to the desired location.
4. Release the mouse button.
To stretch (or scale) the Plane about the plane’s center with the
mouse:
1. Place the mouse pointer over any of the corners.
2. Click (and hold) the left mouse button.
3. Drag the corner to the desired location.
4. Release the mouse button.

Z

Y

X

To rubber-band a corner of the plane tool (while the opposite corner
stays fixed), do the same as above, but hold the Ctrl key down as you
click and drag a corner.
To rotate the Plane tool with the mouse:
1. Place the mouse pointer over one of the axis labels (X, Y, or Z).
2. Click and drag to the desired orientation. Grabbing the X (Y) label
will rotate around the plane’s Y (X) axis. Grabbing the Z label
enables free rotation about the Plane’s center point.
Note that the mouse pointer will change when it is over a hotpoint (if you are in Part or
Frame mode).
(Undo/Redo button at the bottom of screen can be used to undo/redo the tool
transformation)

Plane moving is restricted to the plane perpendicular to your line of sight. If you need to move the Plane in another
plane, rotate the model such that the desired translation plane is perpendicular to your new line of sight. (Note that
the Plane will not exactly track the location of the mouse pointer.)

Page 169

To position the Plane on a part (by specifying three points) with the ‘p’ key:
1. Click the Pick button in the global area above the
graphics window on the desktop.
2. Select “Pick plane tool location > Using 3 points”
from the pop-up menu.
3. In the Graphics Window, place the mouse pointer on
a part and press the ‘p’ key (or whatever mouse
button you have set for the “Selected Pick Action” in
Edit > Preferences > Mouse and Keyboard).
4. Repeat two more times. Note that you are not
specifying corner points – just three unique points.
You can also position the Plane Tool by picking three nodes (this differs from the above where 3 points in space are
used - in that the node ids of the three closest nodes are found and saved). The Plane orientation will be changed
such that it lies in the plane of the three nodes chosen, and will continue to lie in the plane of these three nodes, even
if they change location.
To position the Plane (by specifying three nodes):
1. Click the Pick button in the global area above the
graphics window on the desktop.
2. Select “Pick plane tool location > Using 3 nodes”
from the pop-up menu.
3. In the Graphics Window, place the mouse pointer on
a part, near a desired node and press the ‘p’ key (or
whatever mouse button you have set for the
“Selected Pick Action” in Edit > Preferences > Mouse
and Keyboard).
4. Repeat two more times. Note that you are not
specifying corner points – just three unique
nodes.
If you open the Transformation Editor, and choose
Editor Function > Tools > Plane, you can see the id of
the three nodes that you have chosen.

Page 170

You can also position the Plane Tool by tracing out a line on the screen. The Plane orientation will be changed such
that it is both parallel to the specified line and perpendicular to the screen.
To position the Plane (by specifying a line):
1. Click the Pick button in the global area above the
graphics window on the desktop.
2. Select “Pick plane tool location > Using 2 points”
from the pop-up menu.
3. Move the mouse pointer into the Graphics Window
and press the ‘p’ key. Place the pointer over the
desired starting point. Click and hold the left mouse
button as you trace out the desired line.
4. Release the mouse button.

You can also position the Plane Tool by picking an origin, then a point out on the normal. This takes two picking
operations to accomplish.
To position the Plane (by picking origin, then point on normal):
1. Click the Pick button in the global area above the
graphics window on the desktop.
2. Select “Pick plane tool location > Origin” from the
pop-up menu.
3. Move the mouse pointer into the Graphics Window
and place the pointer over the desired origin of the
plane tool - then press the ‘p’ key.
4. Select “Pick plane tool location > Normal” from the
pop-up menu.
5. Place the pointer over a point along the normal
vector (from the origin of the plane tool) - then press
the ‘p’ key.

Page 171

To set the Plane by specifying parameters exactly:
1. Open the Transformation Editor dialog from
the desktop by clicking Transf...
2. Select Editor Function > Tools > Plane.

3. Enter the desired coordinates for the origin,
the components of the normal vector, and
the x and y size, and press return.
– OR –
3. Enter the id of three nodes and press
return.
– OR –
3. Enter the plane equation parameters (Ax +
By + Cz = D) and press return.
– OR –
3. Enter the desired coordinates for three
corner points into the X, Y, and Z fields and
press return.

You can also rotate, translate, or scale the Plane by selecting the desired transform action, setting the desired axis
and manipulating the slider bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit
of the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Plane since the X,Y,Z numeric
values always update to reflect the current location. If you are positioning the Plane interactively with the mouse, the
values will update when the mouse button is released.
The Undo/Redo button at the bottom of screen can be used to undo/redo the tool transformation.

Shortcut
In Part Mode, right click on center selection point of the line tool. You can do quick x or y rotates, increase or
decrease the size of the tool, hide the tool, or open the transformation editor. You can also use this right click to
quickly create a plane clip, or do a particle streamline trace with the plane tool as the emitter.

ADVANCED USAGE
After a model has been loaded, the initial location of the Plane center is set to the “look-at” point – the geometric
center of all visible geometry and parallel to the X-Y plane. The coordinates of the Plane are specified with respect to
the default frame: frame 0. However, if you have created additional frames, you can position the Plane relative to the

Page 172

origin of a different frame. This is accomplished by selecting the desired frame in the “Which Frame” list in the
Transformation Editor dialog.
You can easily reset the position and orientation of the Plane tool to the default. See How To Reset Tools and
Viewports for more information.
By default the plane tool will be displayed in line mode. You can display the tool as a transparent plane by changing
the setting for Edit > Preferences... View - Plane Tool Filled.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Cursor, Line, Box, Cylinder, Sphere, Cone, Surface of Revolution. See the How To article on
Frames for additional information on how frames effect tools.
The Plane Tool is also used to specify the location of the clip plane for Auxiliary Clipping.
User Manual: Tools Menu Functions

Page 173

Use the Box Tool

INTRODUCTION
EnSight provides a hexahedron shaped specification tool called the “Box” tool. When visible, the Box tool appears as
a (typically white) wireframe box icon with a triad at one corner. The Box tool is used to supply EnSight with a 3D
volume specification, for example to specify the location for a box clip or cut.

BASIC OPERATION
In many cases, the Box tool will automatically turn on when performing some function that requires it. You can also
turn the tool on and off manually by toggling Tools > Box.

The Box tool can be placed in two ways: interactively through direct manipulation of tool “hotpoints” with the mouse or
precisely positioned by typing coordinates into a dialog.
To move the Box Tool with the mouse:
1. Place the mouse pointer over the origin corner
of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Box to the desired location.
4. Release the mouse button.
To stretch the Box Tool with the mouse:
1. Place the mouse pointer over any of the corner
points (except the origin).
2. Click (and hold) the left mouse button.
3. Drag the endpoint to produce the desired
stretched size.
4. Release the mouse button.
To rotate the Box Tool with the mouse:
1. Place the mouse pointer over the center of the
x, y, or z edge(not at the endpoints).
2. Click and drag to rotate.
Note: Selection of the X axis edge will rotate the
box about the Y axis edge. Selection of the Y
axis edge will rotate about the X axis edge.
Selection about the Z axis edge will rotate
about the origin.
Note that the mouse pointer will change when it is over a
hotpoint (if you are in Part or Frame mode).
(Undo/Redo button at the bottom of screen can be used to
undo/redo the tool transformation)

Box tool moving and stretching is in 3 space. (Note the Box may not exactly track the location of the mouse pointer.)

Page 174

To set the Box Tool by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.
2. Select Editor Function > Tools > Box.

3. To place and size, enter the desired
coordinates for the Origin corner and
the length in each of the directions,
and press return.
4. To orient, enter the components of the
orthogonal axis orientation vectors

You can also rotate, translate or stretch the Box Tool by selecting the desired Transform Action, setting the desired
axis, and then manipulating the slider bar. For these tool actions, the values in the “Scale Settings” section control the
sensitivity and limit of the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Box Tool since the numeric values
always update to reflect the current location, size, and orientation. If you are positioning the Box Tool interactively with
the mouse, the values will update when the mouse button is released.

Shortcut
In Part Mode, right click on center selection point of the Box tool. You can do quick hide the tool, or open the
transformation editor.

ADVANCED USAGE
After a model has been loaded, the initial location of the Box Tool is centered about the “look-at” point – the geometric
center of all visible geometry - and is aligned with the model axis system. The coordinates of the Cylinder are
specified with respect to the default frame: frame 0. However, if you have created additional frames, you can position
the Box Tool relative to the origin of a different frame. This is accomplished by selecting the desired frame in the
“Which Frame” list in the Transformation Editor dialog.
You can easily reset the position and orientation of the Box tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

Page 175

SEE ALSO
Other tools: Cursor, Line, Plane, Cylinder, Sphere, Cone, Surface of Revolution. See the How To article on
Frames for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 176

Use the Cylinder Tool

INTRODUCTION
EnSight provides a cylindrical specification tool called the “Cylinder” tool. When visible, the Cylinder tool appears as a
(typically white) cylinder icon with a line running down the central axis. An axis triad will be at the center of the central
axis line. The Cylinder tool is used to supply EnSight with a cylindrical specification, for example to specify the
location for a cylinder clip or cut.

BASIC OPERATION
In many cases, the Cylinder tool will automatically turn on when performing some function that requires it. You can
also turn the tool on and off manually by toggling Tools > Quadric > Cylinder.

The Cylinder tool can be placed in two ways: interactively through direct manipulation of tool “hotpoints” with the
mouse or precisely positioned by typing coordinates into a dialog.
To move the Cylinder with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Cylinder to the desired location.
4. Release the mouse button.
To stretch the Cylinder with the mouse:
1. Place the mouse pointer over either of the center line’s
endpoints.
2. Click (and hold) the left mouse button.
3. Drag the endpoint to the desired location.
4. Release the mouse button.
To change the Cylinder radius with the mouse:
1. Place the mouse pointer over the center ring.
2. Click and drag to the desired radius.
3. Release the mouse button.
To rotate the Cylinder with the mouse:
1. Place the mouse pointer over the end of one of the
central axes.
2. Click and drag until desired rotation is accomplished.
3. Release the mouse button.
Note:
Selecting the x axis will rotate about the Y axis.
Selecting the y axis will rotate about the X axis.
Selecting the z axis will rotate in general about the axis
origin.

Note that the mouse pointer will change when it is over a
hotpoint (if in Part or Frame mode).
(Undo/Redo button at the bottom of screen can be used
to undo/redo the tool transformation)

Page 177

Cylinder moving and stretching with the mouse is restricted to the plane perpendicular to your line of sight. If you
need to move the Cylinder in another plane, either rotate the model such that the desired translation plane is
perpendicular to your new line of sight or use the other modes for manipulating the tool. (Note that the Cylinder will
not exactly track the location of the mouse pointer.)
To set the Cylinder by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.
2. Select Editor Function > Tools > Cylinder.

3. Enter the desired coordinates for the
Origin (location of the center point),
the Axis (direction vector), and the
Radius and press return.

You can also rotate, translate, or scale the Cylinder by setting the desired transform action and axis and manipulating
the slider bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit of the slider
action.
Note that you can also use this dialog to view (rather than set) the position of the Cylinder since the numeric values
always update to reflect the current location. If you are positioning the Cylinder interactively with the mouse, the
values will update when the mouse button is released.

ADVANCED USAGE
After a model has been loaded, the initial location of the Cylinder center is set to the “look-at” point – the geometric
center of all visible geometry and aligned with the X axis. The coordinates of the Cylinder are specified with respect
to the default frame: frame 0. However, if you have created additional frames, you can position the Cylinder relative
to the origin of a different frame. This is accomplished by selecting the desired frame in the “Which Frame” list in the
Transformation Editor dialog.
You can easily reset the position and orientation of the Cylinder tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Cursor, Line, Plane, Box, Sphere, Cone, Surface of Revolution. See the How To article on Frames
for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 178

Use the Sphere Tool

INTRODUCTION
EnSight provides a spherical specification tool called the “Sphere” tool. When visible, the Sphere tool appears as a
(typically white) sphere icon with a line running down the central axis. An axis triad will be at the center of the central
axis line. The Sphere tool is used to supply EnSight with a spherical specification, for example to specify the location
for a sphere clip or cut.

BASIC OPERATION
In many cases, the Sphere tool will automatically turn on when performing some function that requires it. You can
also turn the tool on and off manually by toggling Tools > Quadric > Sphere.

The Sphere tool can be placed in two ways: interactively through direct manipulation of tool “hotpoints” with the
mouse or precisely positioned by typing coordinates into a dialog.
To move the Sphere with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Sphere to the desired location.
4. Release the mouse button.
To stretch the Sphere with the mouse:
1. Place the mouse pointer over either of the center line’s
endpoints.
2. Click (and hold) the left mouse button.
3. Drag the endpoint to the desired location.
4. Release the mouse button.
To rotate the sphere with the mouse:
1. Place the mouse pointer over the end of one of the
central axes.
2. Click and drag until desired rotation is accomplished.
3. Release the mouse button.
Note:
Selecting the x axis will rotate about the Y axis.
Selecting the y axis will rotate about the X axis.
Selecting the z axis will rotate in general about the axis origin.
Note that the mouse pointer will change when it is over a hotpoint (if in Part or Frame mode).
(Undo/Redo button at the bottom of screen can be used to undo/redo the tool transformation)

Sphere moving and stretching is restricted to the plane perpendicular to your line of sight. If you need to move the
Sphere in another plane, either rotate the model such that the desired translation plane is perpendicular to your new
line of sight or use the other modes for manipulating the tool. (Note that the Sphere will not exactly track the location
of the mouse pointer.)

Page 179

To set the Sphere by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.

2. Select Editor Function > Tools > Sphere.

3. Enter the desired coordinates for the
Origin (location of the center point),
the Axis (direction vector), and/or the
Radius and press return.
if you are going to create a developed surface from
a spherical clip, you need to be aware of how the
spherical axis orientation affects this operation.
(See How To Create a Developed Surface)
You can also rotate, translate or scale the Sphere by setting the desired transform action and axis and manipulating
the slider bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit of the slider
action.
Note that you can also use this dialog to view (rather than set) the position of the Sphere since the numeric values
always update to reflect the current location. If you are positioning the Sphere interactively with the mouse, the
values will update when the mouse button is released.

ADVANCED USAGE
After a model has been loaded, the initial location of the Sphere center is set to the “look-at” point – the geometric
center of all visible geometry and aligned with the X axis. The coordinates of the Sphere are specified with respect to
the default frame: frame 0. However, if you have created additional frames, you can position the Sphere relative to
the origin of a different frame. This is accomplished by selecting the desired frame in the “Which Frame” list in the
Transformation Editor dialog.
You can easily reset the position and orientation of the Sphere tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Cursor, Line, Plane, Box, Cylinder, Cone, Surface of Revolution. See the How To article on Frames
for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 180

Use the Cone Tool

INTRODUCTION
EnSight provides a conical specification tool called the “Cone” tool. When visible, the Cone tool appears as a
(typically white) cone icon with a line running down the center axis. The Cone tool is used to supply EnSight with a
conical specification, for example to specify the location for a conical clip or cut.

BASIC OPERATION
In many cases, the Cone tool will automatically turn on when performing some function that requires it. You can also
turn the tool on and off manually by toggling Tools > Quadric > Cone.

The Cone tool can be placed in two ways: interactively through direct manipulation of tool “hotpoints” with the mouse
or precisely positioned by typing coordinates into a dialog.
To move the Cone with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the Cone to the desired location.
4. Release the mouse button.
To stretch the Cone with the mouse:
1. Place the mouse pointer over either of the center line’s endpoints.
2. Click (and hold) the left mouse button.
3. Drag the endpoint to the desired location.
4. Release the mouse button.
To change the Cone radius with the mouse:
1. Place the mouse pointer over the base ring.
2. Click and drag to the desired radius.
To rotate the Cone with the mouse:
1. Place the mouse pointer over the end of one of the central
axes.
2. Click and drag until desired rotation is accomplished.
3. Release the mouse button.
Note:
Selecting the x axis will rotate about the Y axis.
Selecting the y axis will rotate about the X axis.
Selecting the z axis will rotate in general about the axis origin.

Note that the mouse pointer will change when it
is over a hotpoint (if in Part or Frame mode).
(Undo/Redo button at the bottom of screen can
be used to undo/redo the tool transformation)

Cone moving and stretching is restricted to the plane perpendicular to your line of sight. If you need to move the Cone
in another plane, either rotate the model such that the desired translation plane is perpendicular to your new line of
sight or use the other modes for manipulating the tool. (Note that the Cone will not exactly track the location of the
mouse pointer.)
Page 181

To set the Cone by specifying coordinates:
1. Open the Transformation Editor dialog by
clicking Transf... on the desktop.

2. Select Editor Function > Tools > Cone.

3. Enter the desired coordinates for the
Origin (location of the cone tip), the
Axis (direction vector), and the
conical half angle (in degrees) and
press return.

You can also rotate, translate or scale the Cone by setting the desired transform action and axis and manipulating the
slider bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit of the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Cone since the numeric values
always update to reflect the current location. If you are positioning the Cone interactively with the mouse, the values
will update when the mouse button is released.
The clip/cut from the cone tool will extend infinitely from the tip outwards. To limit the extent of the cone clip/cut, use
the plane tool and cut the cone clip/cut as desired.

ADVANCED USAGE
After a model has been loaded, the initial location of the Cone center is set to the “look-at” point – the geometric
center of all visible geometry and aligned with the X axis. The coordinates of the Cone are specified with respect to
the default frame: frame 0. However, if you have created additional frames, you can position the Cone relative to the
origin of a different frame. This is accomplished by selecting the desired frame in the “Which Frame” list in the
Transformation Editor dialog.
You can easily reset the position and orientation of the Cone tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Cursor, Line, Plane, Box, Cylinder, Sphere, Surface of Revolution. See the How To article on
Frames for additional information on how frames effect tools.
User Manual: Tools Menu Functions

Page 182

Use the Surface of Revolution Tool

INTRODUCTION
EnSight provides a surface of revolution specification tool called the “Revolution” tool. When visible, the Revolution
tool appears as a (typically white) icon with a line running down the center axis. By default, the distance of five
planar points from the central axis defines the profile curve of the revolution surface (although you can add points up
to a maximum of ten). The Revolution tool is used to supply EnSight with a surface of revolution specification, for
example to specify the location for a revolution clip or cut.

BASIC OPERATION
In many cases, the Revolution tool will automatically turn on when performing some function that requires it. You can
also turn the tool on and off manually by toggling Tools > Quadric > Revolution.

The Revolution tool can be placed in two ways: interactively through direct manipulation of tool “hotpoints” with the
mouse or precisely positioned by typing coordinates into a dialog.
To move the Revolution tool with the mouse:
1. Place the mouse pointer over the center of the tool.
2. Click (and hold) the left mouse button.
3. Drag the tool to the desired location.
4. Release the mouse button.
To reorient the Revolution tool with the mouse:
1. Place the mouse pointer over either of the center line’s
endpoints.
2. Click (and hold) the left mouse button.
3. Drag the endpoint to achieve the desired orientation.
4. Release the mouse button.
To rotate the Revolution tool with the mouse:
1. Place the mouse pointer over the end of one of the central
axes.
2. Click and drag until desired rotation is accomplished.
3. Release the mouse button.
Note:
Selecting the x axis will rotate about the Y axis.
Selecting the y axis will rotate about the X axis.
Selecting the z axis will rotate in general about the axis origin.

Note that the mouse pointer will change when it
is over a hotpoint (if in Part or Frame mode).
(Undo/Redo button at the bottom of screen can
be used to undo/redo the tool transformation)

Revolution tool moving and stretching is restricted to the plane perpendicular to your line of sight. If you need to move
the Revolution tool in another plane, either rotate the model such that the desired translation plane is perpendicular to
your new line of sight or use the other modes to manipulate the tool. (Note that the Revolution tool will not exactly
track the location of the mouse pointer.)
Page 183

To set the Revolution tool by specifying coordinates:
1. Open the Transformations dialog by
clicking Transf... on the desktop.
2. Select Editor Function > Tools >
Revolution.
The dialog displays the profile curve as a series
of connected line segments with stars
positioned at the curve points. You can edit the
curve by clicking and dragging the points or by
manually entering distance-radius pairs. You
can also add or delete points. As you make
changes, the tool in the graphics window
updates interactively.
To edit points with the mouse:
1. Click on the point and drag to the desired
location.
To add points (up to a maximum of 10):
1. Click Add Point.
2. Move the mouse pointer into the curve
window and click the left mouse button in
the location of the desired new point.
Clicking Delete Point will remove the
currently selected point.
To manually edit a point:
1. Click the point (to select it) in the curve
window or click the desired point in
either the Distance or Radius lists.
2. The distance and radius of the selected
point are shown in the text fields below
each list.
3. Edit the point’s distance and/or radius
value and press return.
To edit the position or orientation:
1. Enter the desired coordinates for the
Origin (location of the axis center point)
or Axis (direction vector) and press
return.
You can also rotate, translate, and scale the Revolution tool by setting the desired transform action and axis and
manipulating the slider bar. In this case, the values in the “Scale Settings” section control the sensitivity and limit of
the slider action.
Note that you can also use this dialog to view (rather than set) the position of the Revolution tool since the numeric
values always update to reflect the current location. If you are positioning the Revolution tool interactively with the
mouse, the values will update when the mouse button is released.

Page 184

ADVANCED USAGE
After a model has been loaded, the initial location of the Revolution tool center is set to the “look-at” point – the
geometric center of all visible geometry and aligned with the X axis. The coordinates of the Revolution tool are
specified with respect to the default frame: frame 0. However, if you have created additional frames, you can position
the Revolution tool relative to the origin of a different frame. This is accomplished by selecting the desired frame in
the “Which Frame” list in the Transformations dialog.
You can easily reset the position and orientation of the Revolution tool to the default. See How To Reset Tools and
Viewports for more information.
Positioning a 3D tool with a 2D device (the mouse) can be difficult. Multiple viewports are sometimes helpful in
positioning tools since you can see the tool simultaneously from multiple vantage points.

SEE ALSO
Other tools: Cursor, Line, Plane, Box, Cylinder, Sphere, Cone. See the How To article on Frames for additional
information on how frames effect tools.

Page 185

Use the Selection Tool

INTRODUCTION
EnSight provides a 2D screen selection tool called the “Selection” tool or “Region Selector”. It is different than most of
the other tools - in that it is not used to create other parts. It is basically used for selection purposes. For example, it
can be used to select a screen region to zoom in to. It can be used in the part selection process. And it can be used
for the element blanking operation.

BASIC OPERATION
Zoom to Region
To use the selection tool to perform a zoom operation:
1. Click the Selection tool
rubberband positioning button.

2. Click in the graphics window
(to set one corner) and drag (to
set the opposite corner) to place
the selection tool.
3. Fine tune the location of the
tool, if needed, by the methods
described below.
4. Click the Zoom symbol, at the
upper left of the tool, to cause
the zoom to occur.
Note: the Undo button is useful if
you want to undo the last
transformation.

You manipulate the tool by:
- clicking and dragging on any
corner to rubberband the tool.
- clicking and dragging on the
center of the tool to move it.
Note: the dotted box indicates the
actual region being used. It is
preserving the aspect ratio.

Page 186

Element Blanking
The selection tool can be used in the element blanking operation.:
1. Select the part(s) on which to do element
blanking.
2. Click on the Selection tool icon to turn on the
tool.
3. Position the tool as desired.
4. Click on the element blanking symbol at the
upper left of the tool.
Note, in order for this to work, the Element blanking
allowed toggle needs to be on (the default).
To undo the blanking, click the Clear or Clear all
parts button.

Results in the following:

Page 187

Part Selection
To use the tool in the part selection process:

1. Turn on the selection tool by clicking the icon.
2. Manipulate the tool until at least some portion of the desired parts
are contained within the tool’s dotted area.
3. Click the Select... button and select “Region”
Note that the selected parts will now be highlighted in the parts list.

SEE ALSO
How To Do Element Blanking
How To Rotate, Zoom, Translate, Scale
User Manual: Tools Menu Functions

Page 188

Use the Spline Tool

INTRODUCTION
Splines can be used for (a) the path of a camera, (b) the path of a clip plane, and (c) the input to a distance vs.
variable query. Splines can be defined and edited as well as saved and restored from disk. Further, the splines have
attributes such as visibility, line width, and color in order to more easily select and manipulate them.
The splines are defined as piece-wise cubic. The spline is thus always guaranteed to pass through the control points
which you define. The definition of the control points can come from a part (such as a particle trace perhaps), be
picked in the graphics window, be input via x/y/z coordinates, or from the position of the cursor tool.

BASIC OPERATION
There are several ways to define a spline and it’s control points:

To create a spline via picking on surfaces:
1. Click the Pick button in the global area above the graphics
window on the desktop
2. Select "Pick spline control point" from the pop-up menu
3. In the Graphics Window, place the mouse pointer on a part
near a desired location and press the "p" key (or whatever
mouse button you have set for the "Selected Pick Action" in
Edit->Preferences->Mouse and Keyboard). A spline control
point marker will appear where you pressed the "p" key. If
more than one control point has been created you will also
see the spline being constructed.

Page 189

To create a spline via the Transformation editor dialog
1. Open the Transformation Editor dialog from the
desktop by clicking Transf...
2. Select Editor Function > Tools > Spline
3. Select New to create a new spline and if you wish,
rename it by editing the Description
4. If you want to create control points from all of the
coordinates of a 1D part, select the part in the part list
and then select Create from selected part(s).
OR
4. If you know the exact location for the control point
select New(at cursor) then edit the X/Y/Z fields to reflect
the correct control point location.
OR
4. Select an existing control point in the Points list. Select
the Copy button. Then select the line in the Points list
after which you want to insert a new point and select the
Paste button.
To edit the control points of a spline:
1. Move the mouse pointer to a control point you wish to
move in the Graphics Window. Click and drag the
control point.
OR
1. Select the point from the Points list and edit it via the
XY/Z fields
OR
1. Select the point(s) you wish to edit and select the
Offset.. button
2. In the resulting pop-up enter a delta x/y/z value to add
to all of the selected points.
Control point(s) can be deleted by:
1. Select one or more points in the Points list
2. Select the Delete button
To edit the spline attributes
1. The Visible toggle will turn the spline on/off in all
viewports (there are no per-viewport controls)
2. You may choose to show the control points. If visible
then the size of the control point glyph is controlled
here.
3. Adjust the Line width and Color here
4. Invert the spline (to use it in reverse).

ADVANCED USAGE
The spline by definition starts at the first control point (spline value of 0.) and ends at the last control point (spline
value of 1). If the spline is used for camera, clip plane path, or distance vs. variable query the direction along the
spline is always in the positive direction. If you wish to use the spline in reverse you simply Invert the spline.

SEE ALSO
Create Clip Splines

Page 190

Visualize Data
Introduction to Part Creation

INTRODUCTION
Much of the strength of EnSight derives from it’s flexible and powerful part creation mechanism. Since virtually every
task you perform in EnSight will involve some form of part manipulation, it is vital to understand these concepts.
In EnSight, a part is a named collection of elements (or cells) and associated nodes. The nodes may have zero or
more variables (such as pressure or stress) currently defined at the node positions. All components of a part share
the same set of attributes (such as color or line width).
Parts are either built during the loading process (based on your computational mesh and associated surfaces) or
created during an EnSight session. Parts created during loading are called model parts. Model parts can also be
created during an EnSight session by performing a copy on other model parts.
All other parts are created during an EnSight session and are called created or derived parts. Created parts are built
using one or more other parts as the parent parts. The created parts are said to depend on the parent parts. If one or
more of the parent parts change, all parts depending on those parent parts are automatically recalculated and
redisplayed to reflect the change. As an example, consider the following case. A clipping plane is created through
some 3D computational domain and a contour is created on the clipping plane. The contour’s parent is the clipping
plane, and the clipping plane’s parent is the 3D domain. If the 3D domain is changed (e.g. the time step changes),
the clipping plane will first be recalculated, followed by the contour. In this way, part coherence is maintained.
This article is divided into the following sections:
The Parts List
Part Attributes

Creating Parts
Part Types
Where Parts Are Created and Maintained

Part Operations
Hints and Tips

The Parts List
Both model parts as well as all derived parts are displayed as items in the Parts List. There are several ways that the
Parts list can be displayed, the default looks something like:
Case number (important when
multiple datasets have been
loaded)
P indicates Parent of
currently selected part
Part numbers
Currently selected part
Part description

The List... button gives you control over many other ways
to display the parts in the Part list - including the order,
whether parent child hierarchy is to be shown, and
whether other details will be shown.

Page 191

This shows the same part list as before, but using the
parent/child tree - which quickly and efficiently shows
the parent of each part.

There are several ways to
easily select multiple parts.
Selected parts can be deleted here.

For models with many parts, the large
part list can be used - which will expand
the list down the left side of the desktop.

If you right click on a selected part (or parts) in the part list, you
have access to a number of part operations

Page 192

Also, Items in the Parts List are selected using standard Motif methods:
To ...

Do this ...

Details ...

Select an item

Select
(or single-click)

Place the mouse pointer over the item and click the left mouse button. The item is
highlighted to reflect the “selected” state.

Extend a contiguous
selection

Select-drag

Place the mouse pointer over the first item. Click and hold the left mouse button as
you drag over the remaining items to be selected. Only contiguous items may be
selected in this fashion.

Extend a (possibly long)
contiguous selection

Shift-click

Select the first item. Place the mouse pointer over the last item in the list to be
selected. Press the shift key and click the left mouse button. This action will
extend a selection to include all those items sequentially listed between the first
selection and this one.

Extend a non-contiguous
selection

Control-click

Place the mouse pointer over the item. Press the control key and click the left
mouse button. This action will extend a selection by adding the new item, but not
those in-between any previously selected items.

De-select an item

Control-click

Place the mouse pointer over the selected item. Press the control key and click the
left mouse button. This action will de-select the item.

Open the Quick
Double-click
Interaction Area for a part

Place the mouse pointer over the item and click the left mouse button twice in rapid
succession.

Creating Parts
The mechanism for creating derived parts is largely the same regardless of part type:
1. In the Parts List, select the part(s) to use as parents.
2. Click the desired feature icon. This will open the corresponding creation section for the part type in the Quick
Interaction area.
3. If necessary, select a variable to use from the Variables List (e.g. for contours or isosurfaces).
4. Set the desired creation attributes in the Quick Interaction area. IMPORTANT: if you change a text field, you must
press return to have the change take effect!
5. Click the Create button in the Quick Interaction area.
The example below shows Isosurface part creation:
2. Click the isosurface
creation icon.

1. Select the parent part(s).

4. Select an appropriate isovalue.
(Often there is a sensible default)

3. Select the variable to use.
5. Click “Create”.

Page 193

Part Types
The following table provides information on the available part types in EnSight:
Part Type

Symbol

Feature Icon

Description

Clip

2

A surface or line resulting from a clip of parts using an IJK, XYZ, or
RTZ surface of the parts; or a clip of other parts using the Line,
Plane, Box, Cylinder, Sphere, Cone, or Surface of Revolution tool;
or a clip of other parts by revolving an existing 1D part.

Contour

C

Lines of constant value on 2D elements.

Developed
Surface

D

A planar surface derived by unrolling a surface of revolution (e.g.
unrolling a clip created with the Cylinder tool).

Elevated Surface

E

A part created by scaling a 2D part (in the direction of the local
surface normal) based on the value of a variable.

Isosurface

I

A surface of constant value through 3D elements.

Model

M

An original part (i.e.loaded from a disk file) or created through some
operation (e.g. copy or extract) on a model part.

Particle Trace

T

A part consisting of the paths taken by one or more massless
particles as integrated through a vector (typically velocity) field.

Profile

P

Plot of a variable along a line (the 2D counterpart to an elevated
surface).

Vector Arrow

V

A part consisting of a set of arrows showing direction and
magnitude of a vector variable.

Subset

S

A part created by node and/or element label range(s) from model
part(s).

Tensor Glyph

G

A part consisting of tensor glyphs showing direction and relative
magnitude of the eigenvectors of a tensor variable.

Material Part

A

A part created according to the intersection of or domains of
material values.

Vortex Core

X

A part consisting of line segments down the center of flow vortices.

Shock Surface/
Region

K

A part consisting of the surface or volume elements where shock is
higher than a threshold.

Separation/
Attachment Line

L

A part consisting of line segments on a surface where flow
separation and attachment is occurring.

Page 194

Part Operations
EnSight provides several powerful part operators. These operations are accessible from the Edit > Part submenu.
Copy

The copy operation creates a dependent copy of another part. The part is created on the client and
is not known to the server. The new part has its own set of attributes (except for representation), but
shares geometric and variable data with the original.
One of the best reasons to create a copy is to show multiple variables on one part at the same time
in a side-by-side configuration. The copies can be moved independently since each new copy is
automatically assigned a new frame.
See How To Copy a Part for more information.

Group

This operation will collapse the selected parts into a new “umbrella” part. Grouping is most often
used to combine a series of parts into a single part for ease in handling. The part is created on the
client and is not known to the server. The operation is reversible through the Ungroup command.
See How To Group Parts for more information.

Delete

The delete operation completely removes not only the currently selected parts, but also any parts
derived from the selected parts.
See How To Delete a Part for more information.

Extract

The extract operation is closely tied to part representations. Extract creates a new dependent part
using only the geometry of the current representation of the part. For example, if the current
representation of a part consisting of 3D elements is Border, the result of extraction will be a part
consisting of all unshared 2D elements (the surface).
Extract is most often used to reduce the amount of information for a part (e.g. for faster display or for
geometry output) or to create a surface shell part – perhaps for subsequent cutting – of a 3D
computational domain.
See How To Extract Part Representations for more information.

Merge

Merge creates one new dependent part from one or more selected parts. The original parts are
unchanged. If only a single part is selected for the operation, merge will create a “true” copy of the
part (as opposed to the “shallow” copy that the Copy operation creates).
Merging is most often used to combine a series of parts into a single part for ease in handling (such
as attribute setting).
See How To Merge Parts for more information.

Part Attributes
All parts have numerous attributes that control behavior and display. Although many attributes can be controlled
either through the Quick Interaction area or the Part Mode icons, complete access is provided by the various Feature
Detail Editor dialogs. Part attributes and the Feature Detail editors are covered in detail in How To Set Attributes.

Page 195

Where Parts Are Created and Maintained
Part creation occurs on either the EnSight client or the server. Since the data that is available on the client and server
are different, it is useful to understand where parts are created and where the data is stored. For example, you can
only perform a query operation for parts that are stored on the server. The following table provides this information
for each part type:
Part Type

Where Created

Data on Server?

Data on Client?

Clip

server

yes

depending on representation

Contour

client

no

yes

Developed Surface

server

yes

depending on representation

Discrete Particle

N/A

yes

depending on representation

Elevated Surface

server

yes

depending on representation

Isosurface

server

yes

depending on representation

N/A

yes

depending on representation

Particle Trace

server

no

yes

Profile

client

no

yes

Vector Arrow

client

no

yes

Subset

server

yes

depending on representation

Tensor Glyph

client

no

yes

Vortex Core

server

yes

depending on representation

Shock Surface/Region

server

yes

depending on representation

Separation/Attachment Line

server

yes

depending on representation

Material

server

yes

depending on representation

Model

In the last column, “depending on representation” means the current visual representation for the part. For
example, if the part’s visual representation is “Not Loaded”, then no data is currently present on the client.

Hints and Tips
With some datasets that contain many parts, it is important to maintain the connection between a part as displayed in
the Graphics Window and the corresponding item in the Parts List. EnSight shows the selected parts as highlighted.
To toggle this feature on or off, click on the Hightlight Selected Parts toggle.

You can rapidly cycle through items in the Parts List using the up/down arrow keys on your keyboard. Select any item
in the list and then press the up arrow (to move to previous entries) or down arrow (to move to subsequent entries).
This is particularly helpful when used in conjunction with the Part(s) Selected Viewport window (as described above)
to quickly locate a part of interest.
You can select parts in the Parts List using a single left click on the part in the graphics window. This should work
unless your single-click settings has been changed from the default Pick Part. To change it back to Pick Part,
Edit>Preferences and click on Mouse and Keyboard.
You can also select parts in the Graphics Window by picking using the ‘p’ key. In Part Mode, select Pick Part from the
Pick pull-down. In the Graphics Window, place the mouse pointer over any portion of the desired part and press the
‘p’ key. If you hold down the control key at the same time, the part is added to the list of currently selected parts.

Page 196

A quick way to create parts using the default settings is to right click on a part in the graphics window. A pulldown
selection will appear that will give you the option to create a Contour, Isosurface or Vector Arrow part using the default
settings using the parent as the part you right clicked.
Selected parts can be written to disk and loaded in a future session. Select File > Save > Geometric Entities ... You
have the option of saving either in EnSight format, VRML format, STL format, or other user-defined formats. See How
To Save Geometric Entities for more information.

SEE ALSO
User Manual: Features, Part Operations

Page 197

Create Contours

INTRODUCTION
A contour is a line of constant value on a two-dimensional (though not necessarily planar) surface. The region on one
side of the line is larger than the isovalue; the region on the other side is less than the isovalue. EnSight creates
contour lines in groups where the isovalues either correspond to the levels in the palette defined for the contour
variable, or a user specified range and distribution. The main level contour lines can also be labeled with the
corresponding palette value.

BASIC OPERATION
2. Click the Contours icon.

1. Select the parent part.

3. Select the variable to use.
4. Click Create.

The Contour Quick Interaction area lets you set the number of contour levels (and sublevels) as well as attach labels
to the contour lines. Contour lines can be synced to the palette levels or can be chosen manually.

If you want the levels of the variable palette to be used for contours:
In the parts list, double-click the contour part you wish to edit.

1. Select the Variable.
2. Toggle on Sync To
Palette.
3. Select the number of
sublevels desired (if
any). And make sure
Visible toggles are set as
desired.
See How To Edit Color Maps for how to set the color
palette levels.
4. Set the Visibility, Spacing, Color, and
Format of the contour labels.
Note that only the main contour levels (not the
sublevels) are labeled.

Page 198

If you want contour levels to be independent of Variable palette levels:
In the parts list, double-click the contour part you wish to edit.

1. Select the Variable.
2. Toggle off Sync To
Palette.
3. Specify the Min and
Max Range.
4. Specify the number
of Levels and
sublevels.
5. Specify the Distribution method for the Range.
6. Set the Visibility, Spacing, Color, and Format of the
contour labels.

Shortcut
In Part Mode, right click on a part in the graphics window. In the resulting pulldown, choose Contour. A window will
pop up to choose a variable. This then automatically creates a contour part with the default settings using the
selected variable and using the right-clicked part as the parent part.

ADVANCED USAGE
When Sync To Palette is specified, the levels of the variable palette are used as the contour levels. You must edit the
palette using the Feature Detail Editor for Variables to modify the number of levels, distribution, etc. See How To
Edit Color Maps for guidance.

OTHER NOTES
The default behavior is to color the contour part by the creation variable. If you toggle this off, the contour part will not
be colored by a variable automatically, but will be white.
Unlike most part creation operators, contours are created from the client’s representation of the part – not the
server’s. If the parent part of the contour consists of one-dimensional elements or has no client-side visual
representation at all, the resulting contour will be empty. This would be the case if the parent part was currently
displayed as feature angle, border representation, or not loaded. The 3D border, 2D full representation is typically
used for contour part parents. See How to Change Visual Representation for more information.

SEE ALSO
Introduction to Part Creation, How To Edit Color Maps.
User Manual: Contour Create/Update

Page 199

Create Isosurfaces

INTRODUCTION
An isosurface is a surface of constant value in a three-dimensional field. It is the 3D counterpart to the contour loop:
the region on one side of the isosurface has values greater than the isovalue; the region on the other side has values
less than the isovalue. In EnSight, an isosurface can be generated from a scalar variable, a component or magnitude
of a vector variable, or a component of the model coordinates.
An isosurface of a scalar or vector variable is typically a complex surface reflecting the distribution of the underlying
variable. Isosurfaces of coordinates, however, are typically regular geometric shapes such as planes, cylinders,
cones or spheres.

BASIC OPERATION
2. Click the Isosurface
creation icon.

1. Select the parent part.

4. Select an appropriate isovalue.
(the default will be a mid-range value)

3. Select the variable to use.
5. Click Create.

Shortcut
In Part Mode, right click on a part in the graphics window. In the resulting pulldown, choose Isosurface. A window will
pop up to choose a variable. This then automatically creates an isosurface part with the default settings using the
selected variable and using the right-clicked part as the parent part.

Page 200

ADVANCED USAGE
Interactive Isosurfaces
You can have EnSight automatically generate and display isosurfaces as you adjust a slider with the mouse.

1. Set the Interactive mode to Manual.

2. Adjust the slider to the desired location.

You can also set the Interactive mode to Auto and EnSight will automatically sweep from Range Min to Max with step
size equal to Increment. Alternatively, you can left click on the isosurface part in the graphics window and grab the
green handle shaped like a “+” and drag it to interactively change the isovalue.

Isosurface Animation
A range of isosurfaces can be automatically generated and viewed in a flipbook. Flipbooks provide on-screen
animation of various dynamic events and (in the default setting) permit graphic manipulation (e.g. rotation or zoom)
while the animation runs.
1. Open the Feature Detail Editor for isosurfaces (Edit > Part Detail Editors > Isosurfaces ...).

2. Select the isosurface part.

3. In the Creation Attributes section, set the
Animation Delta to an appropriate value and hit
return. For each page (frame) of the flipbook,
this value will be added to the current value to
yield the new isovalue.

Page 201

4. Click the Flipbook icon.

6. Set the number of pages
to an appropriate value.

5. Set the Load Type to
Create Data.

7. Click Load.
8. When loading is complete, the flipbook will begin to be displayed. You can then control the various run
options under the Run tab.
EnSight can also automatically calculate a range of isosurfaces during keyframe animation.

Creating Multiple Offset Isosurfaces:
You can have EnSight create multiple isosurfaces at a specified delta value. The results is a group of isosurfaces:
4. Select an appropriate isovalue.
2. Click the Isosurface
(the default will be a mid-range value)
creation icon.

5. Set the number of surfaces and the delta between
them.
1. Select the parent part.

3. Select the variable to use.
6. Click Create.

Isovolume Creation
An isovolume is a volume whose constituents (e.g. nodes and elements) are constrained to a constant interval range
in a scalar field. In EnSight, you can constrain the isovolume to ranges less than an interval minimum, greater than an

Page 202

interval maximum, or between the interval minimum and maximum.
1. Open the Feature Detail Editor for isosurfaces
(either: Edit > Part Detail Editors > Isosurfaces ... ,
or double click the Isosurface Feature Icon).

2. Select the isosurface part.

3. In the Creation Attributes section, set Type to
Isovolume.
4. Set the Constraint to Band to constrain the
isovolume within an appropriate Min and Max
range of the scalar variable.

OTHER NOTES
Effective display of more than two nested isosurfaces is difficult. Set transparency on the outermost isosurface(s) to
reveal the inner surfaces. To avoid confusion, don’t try to display isosurfaces of more than one variable
simultaneously, or multiple isosurfaces of the same variable colored by different variables.

SEE ALSO
How-To Create a Flipbook Animation, How-To Create a Keyframe Animation
User Manual: Isosurface Create/Update

Page 203

Create Particle Traces

INTRODUCTION
Streamline and Pathline Traces:
A particle trace represents the path a particle would take if released in a flow field. From an initial seed point (the
emitter), a path is formed by integrating through the velocity field over time. The path is therefore everywhere parallel
to the flow. Traces calculated using a single time step in a flow field are called streamlines. The path calculated using
a transient flowfield that is updated as the calculation proceeds is known as a pathline.
EnSight provides a great deal of control over emitter definition and trace appearance:
• Emitters can be defined using one of the built-in tools (Cursor, Line, or Plane) or by clicking on any
surface in the Graphics Window. The nodes of an arbitrary part can be used as an emitter, or the emitter
time and locations can be read from a file (see EnSight Particle Emitter File Format in the Chapter 11 of
the User Manual).
• The streamline path can be generated in the positive, negative, or positive and negative time directions.
• Traces can be restricted to lie on any surface to search for flow topology and separation features.
• For transient cases, an emitter can have a delta time that controls the periodic release of additional
particles into the dynamic flow.
• Emitters can be interactive: as you move the emitter with the mouse, the associated traces
automatically recalculate and redisplay (This option is not available for surface-restricted Particle
traces, traces emitted from a Part, in Server of Server mode, nor for Pathlines).
• Trace paths can be displayed as lines, ribbons, or as square tubes, where ribbon or tube twist follows
the local flow rotation around the path.
• Particle traces can be easily animated to provide intuitive comprehension of the flow field. Complete
control over all aspects of the animating tracers is provided, including length, speed, and release
interval for multiple pulses.
Node Tracks:
Another form of trace that is available in EnSight is entitled node tracking. This trace is constructed by connecting the
locations of nodes through time. It is useful for changing geometry or transient displacement models (including
measured particles) which have node ids.
Min/Max Variable Tracks:
A further type of trace that is available is a min or max variable track. This trace is constructed by connecting the min
or max of a chosen variable (for the selected parts) though time. Thus, on transient models one can follow where the
min or max variable location occurs.
Both the node tracking and the min/max variable tracking options are like a connect-the-dots through time trace.

Page 204

BASIC OPERATION
To trace particles through a steady-state flow field (streamline):
2. Click the Particle Traces icon.

1. Select the flow field
mesh part(s) to trace
through.

6. Click Create. The particle traces will be
created from the desired emitter. Their
maximum time duration is controlled via
the Total Time Limit found under Emit...

3. Select Streamline as the type.

4. Select the vector variable to
use.
5. Select the desired emitter.
6. If the emitter is a tool (Cursor, Line, Plane), position the
tool at the desired emitter location. You can also click
the Tool Location button to precisely position the tool.
If the chosen emitter is Part, then enter the part number
in the Part ID field and press return.

The following are the available Emit From options. Note that traces will only be generated for those emitter points
that actually lie within an element of the selected flow field part(s).
Cursor

A single trace will be emitted from the Cursor tool.

Line

Multiple traces will be emitted from evenly spaced points along the Line tool.
Enter the desired number of traces in the # Points field and press return.

Plane

Multiple traces will be emitted from evenly spaced points in a grid pattern over the
Plane tool. Enter the desired number of traces in the X and Y direction (with
respect to the Plane tool’s axis) in the # Points X/Y fields and press return. The
total number of traces will be the product of X and Y.

Part

One trace will be emitted from the number of nodes of the part you specify. This
number of nodes will be randomly selected. Enter the number (from the Main
Parts list) of the part you wish to use as an emitter, and the number of nodes.

File

Traces will be emitted from the locations, and at the times, specified in an EnSight
Particle Emitter file. See EnSight Particle Emitter File Format in Chapter 11 of the
User Manual.

Shortcut
To quickly create a particle trace, right click on a tool (cursor, line or plane) and choose Particle Trace. This will
create streamline trace(s) using default settings and the tool as the emitter. The complete set of particle trace
attributes can be edited in the Feature Detail Editor for Traces. However, some emitter attributes can be changed

Page 205

from the Particle Traces Quick Interaction area by clicking the Emit... button:
Click to set the trace direction:
+: forwards in time (positive
velocity direction) from the
emission point(s)
-: backwards in time (negative
velocity direction) from the
emission point(s) towards the
entering flow boundary
(Streamlines only)
+/-: both forwards and
backwards (Streamlines only)

Toggle on to have start time be
the current time, otherwise specify
the start time (Streamlines only).

Set the total amount of time
a trace will last (it may
terminate for other reasons
as well). An intelligent
default will be set for you.
Solution time at which to
begin pathline trace
(Pathlines only).
Delta emission time for
pathlines. If not zero, a new
set of traces will be emitted
at S, S+D, S+2D, etc. into
the changing flow field
(where S is the Start time
and D is the delta value).
Used to create streaklines
or smoke traces. Animated
streaklines are one of the
most powerful methods for
visualizing transient flow
(Pathlines only)

Display Traces as Ribbons or Square Tubes, and control Arrowheads
Streamline and Pathline Particle paths can be displayed as lines, ribbons, or square tubes, where ribbon or tube twist
follows the local flow rotation. To enable ribbon or square tube display, and change trace arrowheads:
1. Double-click the desired particle trace part in the Main Parts
list (to open the Quick Interaction area for the trace part).
2. Click Show As... to open the Trace Show As Attributes dialog.
3. Set Show As to Ribbon or Square Tubes.
4. If desired, change the default ribbon or square tube width and
press return.
5. Select the Arrowhead representation desired.
(Cone, Normal, or Triangles)
6. Set the number of arrowheads to display along a trace.
7. Set the arrowhead size.
5. Click Close.

Note that node tracks and min/max variable tracks can only be
displayed as lines. Trace arrowheads can be used for tracks, but
this must be done from the Feature Detail Editor (Traces).

Animate Particles
Any type of particle trace can be animated. See How To Animate Particle Traces for more information.

Pick a Surface to Trace a Particle
Rather than emit from a tool or a part, you can also interactively pick points on a surface in the Graphics Window to
define emitter locations. To do this:
1. Execute steps 1-3 as described under Basic Operation above.
2. Click the Pick Surface toggle.

Page 206

3. Click Create.
4. Move the mouse into the Graphics Window and click the left mouse button when the cursor is over the
desired location. The clicked point must be found within some element of the selected flow field mesh
part to result in a trace.
5. You can click to create as many point emitters as you like. When done, move the mouse out of the
Graphics Window.
6. Toggle off the Pick Surface button.
Note that you can also specify a rake (line) or net (plane) emitter by picking on a surface. Just set the emitter to Line
or Plane prior to clicking Create. Then follow in the instructions in the pop-up window.

Interactive Particle Tracing
If a particle trace was created from one of the tool emitters (Cursor, Line, or Plane) and the trace is a streamline trace,
the emitter can be made interactive. When interactive, the tool that created the particle trace part can be moved with
the mouse. As the tool is moved, new particle traces are automatically recalculated and redisplayed (This option is
not available for surface-restricted Particle traces, traces emitted from a Part, in Server of Server mode, nor to
Pathlines). To trace interactively:
1. Either create a particle trace part as described above (based on a tool) or double-click an existing particle
trace part to open the Quick Interaction area for that part.
2. Toggle on Interactive Emitter. If the tool that originally defined the emitter is not visible, it will be turned on
by this operation.
3. Move the mouse into the Graphics Window and manipulate the tool as desired. See the article on the
applicable tool for information on tool manipulation (Cursor, Line, or Plane).
4. When done, toggle off Interactive Emitter.

Page 207

Trace Surface-Restricted Particles
EnSight can trace particles such that they are constrained to lie on a (not necessarily planar) 2D surface – even if the
velocity is zero at the surface. The trace is calculated by projecting a short distance off the surface into the 3D flow
field and using the velocity value found there. Both the projection distance (variable offset) and a display offset are
user definable.
Surface-restricted trace emitters are defined by mouse action in the Graphics Window. When you click and drag over
the desired surface, the emitter is defined by projecting the mouse path onto the surface. To trace surface-restricted
particle traces:

1. Select the desired surface part(s) in the Main Parts list.
This should be the surface you wish to trace on.
2. Set the desired vector variable to use for tracing.
3. Select the desired emitter type (Cursor, Line, or
Plane). Note that the applicable tool will not actually
be used in this operation (a pick action will be used).
4. Toggle on the Surface Restricted button. Note that all
subsequent tracing will be assumed to be surface
restricted until this is toggled off.
5. If the Emit From is set to Line or Plane, enter the
desired number of points (Line) or X and Y points
(Plane).
9. Click the Create button.
10. Move the mouse pointer into the Graphics Window
and:
for a Cursor emitter: click the left mouse button on the
desired location.
for a Line emitter: click and hold the left mouse button
on one endpoint of the desired line. Drag to the other
endpoint (a white line will provide feedback).
for a Plane emitter: click and hold the left mouse button
on one corner of the desired region. Drag to the
opposite corner (a white rectangle will provide
feedback).
11. You can continue to specify emitters of the selected
type as long as the mouse pointer remains in the
Graphics Window. When the pointer exits the window,
the trace part will be created.
12. When done, toggle off Surface Restricted.

Note that this operation can also be done in the Feature Detail Editor for Traces.
In this dialog, you have control over the various other attributes of the trace - including variable offset, display
offset, trace direction, etc.

Page 208

Trace Pathlines
EnSight provides complete control over transient particle tracing. Both the start time and the stop time can be
specified. In addition, you can specify a delta value for an emitter that will cause additional particles to be emitted into
the flow at regular intervals. This type of pathline is also called a streakline or smoke trace.
You create a pathline trace by setting the Type to Path (rather than Stream) prior to clicking Create. By default, the
pathlines will start at the first time step of your simulation and terminate at the last step (unless stopped earlier). You
can change these defaults with the Emission Detail Attributes dialog as described above (click Emit... to open).

Edit Emitter Attributes
Although the Particle Trace Quick Interaction area provides most tracing controls, the Feature Detail Editor for Traces
provides complete control over all creation attributes. To use the editor:
1. Select Edit > Part Feature Detail Editors > Particle Traces... to open the Feature Detail Editor (Traces)
dialog.
2. Select the desired particle trace part in the part list at the top of the dialog.

Set the desired flow field
variable
Set the fraction of each
component of the vector
variable to use in the trace
calculation.

Set ribbon width

Trace type
Line or ribbon display
Number of arrowheads along
the trace.

List of the emitters belonging
to the selected trace part

Set interactive emitter
Set emitter direction, total time

Set to emit at current time, or
set emission time.

Set Arrowhead size.

Emission tool for currently
selected emitter
Number of points (If Line or
Plane emitter)
Add Emit: add a new emitter to
the selected part based on the
current attributes.
Delete Emit: delete the
selected emitter.
Set Total Time to the default.

Set emission start and delta
Toggle on Surface Restricted
tracing

Toggle on surface picking for
emitter definition

Set surface restricted variable
and display offsets.

Page 209

Massed Particle Traces
Ensight also provides massed particle traces via the Feature Detail Editor for Traces.
1. Select Edit > Part Feature Detail Editors >
Particle Traces... to open the Feature Detail
Editor (Traces) dialog.
2. Select the desired the particle trace part in the
part list at the top of the dialog.
3. Click the Massed Particle turn-down to reveal
the massed particle parameters.
4. Modify the massed particle parameters
according to your dataset.
Each term in the momentum balance equation
has a separate tab containing the parameters
which pertain.
5. Toggle on Massed Particles.
The selected particle trace part will update to a
massed particle trace(s) taking into consideration
the parameters you specified.
For the theory used in massed particle traces, see
the User Manual: Particle Trace Create/Update

Page 210

Node Tracks
Ensight provides the capability to track the location of node(s) through time. As one would expect, node ids are
required, and this only makes sense for nodes that change location over time - whether by changing geometry or by
transient displacement. Measured particle parts are often a particularly good choice for this option.
1. Select the part(s) containing the nodes you
wish to track in the main Part list.
2. Set Type to Node track.
3. Optionally you can modify the begin and end
times to use for the track by clicking here.
The default will be all time steps.
4. Specify the particular node id you wish to
track, or do “ALL”.
You can use the ‘Use ALL nodes” button to select
all if you have modified the field.
5. Click Create.

Min/Max Variable Tracks
Ensight provides the capability to track the location of the minimum or maximum of a chosen variable through time.
This of course only makes sense for transient models.
1. Select the part(s) containing the variable, for
which you wish to track the min or max.
2. Set Type to Variable min. track
(Or Variable max. track)
3. Select the desired variable.
4. Optionally you can modify the begin and end
times to use for the track by clicking here.
The default will be all time steps.
5. Click Create.

ADVANCED
From time to time we have users that wish to trace pathlines backward in time. This can be accomplished fairly easily
using the EnSight casefile format. (Note, if your data is in a different format, you can use File->Save->Geometric
Entities to convert it into casefile format).
1. Reverse the order for the timeset files, by using a negative filename increment.
Example:
TIME
time set:
filename start number:
filename increment:
time values:

1
1
1
0.0 2.0 4.0 6.0 8.0

change to:
TIME
time set:
1
filename start number: 5

Page 211

filename increment:
time values:

-1
0.0 2.0 4.0 6.0 8.0

2. Create a vector variable that is the negative of the normal vector field. Simply use the variable caculator to create
a new vector variable (neg_vector = - vector).
3. Create pathlines using the neg_vector variable.

OTHER NOTES
Particle trace calculation can be expensive for large or transient datasets and/or a large number of particles. Be
careful when you initiate a trace operation – there is currently no way to abort it. If you are calculating pathlines, you
should specify as many particles as possible at one time. Much of the pathline execution time is in reading the
transient data from disk and this operation has to be performed regardless of how many traces were specified.
The EnSight particle trace algorithm integrates the vector flow field over time using a 4th-order Runge-Kutta method
with a time varying integration step. Several of the integration parameters can be changed by the user. See Particle
Trace Create/Update in the User Manual for more information.
If you have trace data for other types of particles (e.g. for multi-phase flow simulations) you can use the discrete/
measured data facility to load the particle path positions and animate them over time.

SEE ALSO
How To Animate Particle Traces
User Manual: Particle Trace Create/Update

Page 212

Create Clips

INTRODUCTION
EnSight provides a powerful set of clipping operators. See the following How To articles for more information:
Create Line Clips

Clip lines are linear clips through 2D or 3D models (using the Line Tool) with samples taken at
evenly spaced intervals (grid), or at intersections of element boundaries of the parent parts
(mesh). Clip line values can be visualized using profiles or queried and sent to a plotter.

Create Plane Clips

A clipping plane is a planar slice through a 3D mesh using the Plane Tool. EnSight’s clipping
operation can take arbitrary cuts through either structured or unstructured meshes. The clip
can be infinite in extent (at least to the bounds of the parts it is created from) or restricted to
the bounds of the Plane tool. The nodes of the resulting clipping plane can be based on the
topology and resolution of the underlying mesh or sampled on a regular grid.
You can also create a clip that contains all the elements that intersect the plane value via the
crinkly domain specification. These clips help view the integrity of the mesh at these values.

Create Box Clips

A Box clip is a 3D volumetric hexahedral-shaped clip or cut. This clip uses the box tool (which
can be manipulated anywhere in space), and the result can be the surface intersection of the
box tool walls and the model, the volume portion of the model inside the tool, the volume
portion of the model outside the tool, or the crinkly surface elements of the intersection. Be
aware that due to the algorithm used, this clip can (and most often does) have chamfered
edges, the size of which depends on the coarseness of the model elements.

Create Quadric Clips

In addition to standard clipping planes, EnSight also provides clipping against quadric shapes.
These clips use the corresponding quadric tool (Cylinder, Sphere, Cone, Surface of
Revolution) to specify the location of the clip.
You can also create a clip that contains all the elements that intersect the quadric value via the
crinkly domain specification. These clips help view the integrity of the mesh at these values.

Create IJK Clips

An IJK clip is a 1D or 2D slice through a structured mesh. The resulting clip is a 1D line or 2D
surface where one dimension (e.g. I) is held fixed while the other one or two dimensions (e.g.
J and K) vary. The minimum and maximum range of the free dimensions can be set by the
user, as well as the step size. IJK clips can be interactively animated throughout the range of
the fixed dimension by manipulating a slider.
Although planar clips can still be created through structured meshes, it is often preferable to
create IJK clips since they are faster to calculate and use less memory. In addition, IJK clips
are often more intuitive for the user (who typically built the mesh).

Create XYZ Clips

An XYZ clip is a 1D or 2D slice through a 2D or 3D mesh (structured or unstructured). The
resulting clip is a 1D or 2D mesh slice where one of the dimensions (e.g. X) is held constant
(or fixed) while the other two dimensions (e.g. Y and Z) vary in reference to the local frame of
the mesh. XYZ clips can be interactively animated throughout the range of the fixed
dimension by manipulating a slider. The minimum, maximum, and step size of the range of the
fixed dimension can be set by the user.
Although plane clips can still be created through meshes, it is often preferable to create XYZ
clips since they are constrained to the local frame of the meshed part.
You can also create a clip that contains all the elements that intersect the mesh slice value via
the crinkly domain specification. These clips help view the integrity of the mesh.

Create RTZ Clips

An RTZ clip is a 1D or 2D slice through 2D or 3D meshes (structured or unstructured). The
resulting clip is a 1D or 2D mesh slice where one of the dimensions (e.g. R,”radial
component”) is held constant (or fixed) while the other one or two dimensions (e.g. T, ”theta
component” and Z, “z axis component”) vary in reference to the local frame of the mesh. RTZ
clips can be interactively animated throughout the range of the fixed dimension by
manipulating a slider. The minimum, maximum, and step size of the range of the interactive
fixed dimension can be set by the user.

Revolution Tool Clips

A Revolution Tool clip can be made using the surface of revolution tool. It can be the surface
created by the intersection of the surface of revolution tool and the model, the elements
intersected by the surface of revolution tool (crinkly), or the volume of the inside and/or the
outside domain swept by the revolution tool. This clip cannot be interactively manipulated.

Revolve 1D Part Clips

A Revolution of 1D Part clip can be made using a 1D part and a user specified axis. It can be
the surface created by the intersection of the 1D part about the axis and the model, the
elements intersected by the 1D part about the axis(crinkly), or the volume of the inside and/or
the outside domain swept by the 1D part about the axis. This clip does not have interactive
manipulation capability, with a slider or by dragging the tool with the mouse. However, if the 1D
part is capable of being moved, you can move it and the revolution clip will update.

Create Clip Splines

Spline clips will sample a defined spline on evenly spaced intervals along the spline. Values
along a spline clip can be visualized using profiles or queried and sent to a plotter, or used in
subsequent computations such as computations of a line integral.

Create General
Quadric Clips

A general quadric clip AX2+BY2+CZ2+DXY+EYZ+FXZ+GX+HY+IZ=J can be created. This is
only available from the Clip Feature Detail Editor.

Page 213

Create Clip Lines

INTRODUCTION
In addition to standard clipping planes, EnSight also provides one dimensional clipping. Clip lines are linear clips
through 2D or 3D models with either samples taken at evenly spaced intervals (grid) or true intersections at the faces
of the parent part’s elements (mesh). Values along a clip line can be visualized using profiles or queried and sent to
a plotter.

BASIC OPERATION
2. Click the Clip icon.

1. Select the parent part.

3. Select Line from the Use Tool pull-down.
4. Select Mesh or Grid type.
5. If Mesh, select Finite or Infinite
If Grid, set the number of evenly spaced
points on the line
6. Position the Line tool as
desired (see How To Use the
Line Tool).
7. Click Create.

Note: To quickly create a line clip, right click on the line tool and choose Clip. This will create a
line clip using the default settings.

Page 214

ADVANCED USAGE
Like the other clipping tools in EnSight, clip lines can be interactive: as you drag, rotate, or stretch the Line tool with
the mouse, the clip line is automatically recalculated and re-displayed. If a query has been created from the clip line,
the plotted curve will automatically re-display as well. To perform interactive line clips:
1. Double-click the desired clip line part
in the parts list.

2. Toggle on Interactive Tool in the
Quick Interaction area.

3. Move the mouse into the Graphics Window. Click on one of the Line tool hotpoints (either endpoint
or center axis origin or axes) and drag the tool to the desired location.
Note that the line tool itself will be made invisible while moving the tool interactively, so as not to obscure the
clip. It will reappear when the mouse is released.
.

A line clip can be specified by identifying two nodes as points
on the line.
This requires that node ids be available and is performed in
the Feature Detail Editor (Clips) dialog.
The effect of this method is that the line clip remains tied
to the two nodes, even if their location moves over time.

OTHER NOTES
It is sometimes useful to display just the nodes of a line clip. Using the Feature Detail Editor, you can change the
display such that only nodes (not lines or elements) are displayed. The nodes can be shown as dots, crosses, or
spheres. If displayed as crosses or spheres, the size (radius) can be constant or scaled by the value of a variable.
See How to Set Attributes for more information.

Page 215

SEE ALSO
Introduction to Part Creation
How To Use the Line Tool
How to Create Profile Plots
How to Query/Plot.
Other clips:
How to Create Clip Planes
How to Create Quadric Clips
How to Create Box Clips
How to Create IJK Clips
How to Create XYZ Clips
How to Create RTZ Clips.
User Manual: Clip Create/Update

Page 216

Create Clip Planes

INTRODUCTION
A clipping plane is a planar slice through a 3D mesh. EnSight’s clipping operation can take arbitrary cuts through
either structured or unstructured meshes. The clip can be based on EnSight’s plane tool, and as such can be infinite
in extent (at least to the bounds of the parts it is created from) or restricted to the bounds of the Plane tool. The nodes
of the resulting clipping plane can be based on the topology and resolution of the underlying mesh or sampled on a
regular grid according to the plane tool.
A clip can also be created by specifying the node id of three nodes. When node ids are used, the plane will be infinite
in extent and will stay tied to those three nodes - even if they move in a changing geometry model.
Besides creating the intersection of a plane through a domain, which is the normal mode for clipping, a clipping plane
can also be used to create parts which are what would result from a cut of its parent domain into “front” (inside) and or
“back” (outside) parts. These parts contain valid elements of the same order as the original domain parts.
Like other clip tools, clipping planes can be interactively manipulated with the mouse providing a powerful volume
visualization capability. Clipping planes can also be automatically animated to display results throughout a region of
space or over time.

BASIC OPERATION
2. Click the Clip icon.

1. Select the parent part.

3. Select Plane from the Use Tool pull-down.

4. Position the Plane tool as desired (see
How To Use the Plane Tool).
5. Click Create.

Note: Multiple plane clips with a delta in the normal direction can be created easily by setting these values.

Interactive Clipping Planes
Like the other clipping tools in EnSight, intersection clip planes (based on the plane tool) can be interactive: as you
drag the Plane tool with the mouse, the clipping plane is automatically recalculated and re-displayed. To perform
interactive plane clips:
1. Double-click the desired
clip plane part in the
parts list.

2. Toggle on Interactive
Tool in the Quick
Interaction area.

3. Move the mouse into the Graphics Window. Click on one of the Plane tool
hotpoints (centerpoint or axis labels) and drag the tool to the desired location.

Page 217

ADVANCED USAGE
Using 3 Node Ids
You can specify three nodes on a plane (using their node ids) and clip in an infinite manner. This method of producing a plane clip has the added benefit that the plane will stay tied to those three nodes even if it is a changing geometry model. This method requires the use of the Feature detail editor for clips

1. Select the parent part in the main part list.
2. Double click on the Clip icon to bring up
the Feature Detail Editor (Clips).
3. Enter the id for three nodes that lie on the
desired plane.
4. Hit the create button.

Note: To quickly create a plane clip, right click
on the plane tool and choose Clip. This will
create a plane clip using the default
settings.

Page 218

Attaching a Plane Clip to a Spline
A Clip created with the Plane tool may be attached to a defined spline.
1. Create a spline (How To Use the Spline
Tool)
2. Now, create a clip plane as previously
indicated. Click on the Advanced button in the
Clip Plane quick interaction area to open the Clip
Plane Feature Detail Editor. Select the Clip
Plane part in the Feature Detail Editor
3. Attach the plane clip to a spline by selecting
the desired spline from the pulldown in the Clip
Plane Feature Detail Editor.
4. Adjust the plane clip location (0 to 1) via the
Value input field or the slider.

Page 219

Grid Clips and Finite Clips
By default, clipping planes (based on the plane tool) are calculated based on the resolution and topology of the
underlying mesh (parent part(s)). Clipping planes can also be calculated using a regular sampling of the mesh. Such
a clip is called a grid clip and is typically used for clipping unstructured meshes where element volumes vary widely.
Creating vector arrows on a grid clip typically yields a more useful visualization than on a standard mesh clip.
By default, clipping planes extend to the bounds of the parent part. A clipping plane can also be restricted to the
bounds of the Plane tool.
To change an existing clipping plane to a grid clip or to have finite extent:
1. Double-click the desired clipping plane part in the parts list.

2. To change to a grid clip,
select Grid from the
Plane Type pull-down.

3. To change to a finite-extent clipping plane, select Finite from the Plane
Extents pull-down.

Clipping Plane Animation
Although you can interactively sweep a clipping plane (based on the plane tool) through a volume, it is sometimes
desirable to have EnSight automatically calculate a series of clipping planes for you. These can then be replayed (as
fast as your graphics hardware will permit) using EnSight’s Flipbook Animation facility. The flipbook can animate a
series of clipping planes using a starting and ending position for the Plane tool. You can also use the Keyframe
Animation facility to animate clipping planes.
For a description of calculating a series of clipping planes with the Flipbook, see How To Create a Flipbook
Animation. For more information on keyframing, see How to Create a Keyframe Animation.

Cutting with Planes
A plane can be used to create parts which are the result of a cut of its parent domain into “front” (inside) and or “back”
(outside) parts. These parts contain valid elements of the same order as the original domain parts. Cutting can be
used to slice away portions of a model that are not needed or to create animation effects such as “opening” closed
regions to view the interior.
1. Select the desired parent parts in the parts list.
2. Click the Clip feature
icon.
3. Select the Plane Tool.
4. Set the Domain to
Inside, Outside, or In/
Out (both inside and
outside).
5. Hit the Create button.

Page 220

Crinkly Plane Clips
You can also check the integrity of your mesh by clipping with a crinkly intersection. Specifying a Crinkly Domain
results in a part composed of all the mesh elements that intersect the plane tool.

1. Change the Domain to
Crinkly.

2. Click the Apply Tool
Change button.

OTHER NOTES
If you have a clip defined by three node ids and you attempt to use the interactive mode (which makes no sense for
the 3 node option), the interactive movement of the clip will occur according to the plane tool - but will go back to the
3 node representation when you release the mouse button.
Use clipping planes to create planar clips through arbitrary meshes. If you have a structured mesh (such as those in
PLOT3D format), you may wish to use IJK clips instead. An IJK clip displays a “plane” of constant I, J, or K. An
interactive IJK clip will sweep through the range of (for example) I displaying the JK plane at each I value. See How
to Create IJK Clips for more information.

SEE ALSO
Introduction to Part Creation
How To Use the Plane Tool
How To Create a Flipbook Animation.
Other clips:
How To Create Clip Lines
How To Create IJK Clips
How To Create Quadric Clips
How To Create XYZ Clips
How To Create RTZ Clips
How To Create Box Clips.
How To Use the Spline Tool
User Manual: Clip Create/Update

Page 221

Create Box Clips

INTRODUCTION
A Box clip is a 3D volumetric hexahedral-shaped clip or cut. This clip uses the box tool (which can be manipulated
anywhere in space), and the result can be the surface intersection of the box tool walls and the model, the volume
portion of the model inside the tool, the volume portion of the model outside the tool, or the crinkly surface elements
of the intersection.

Be aware that due to the algorithm used, this clip can (and most often does) have
chamfered edges, the size of which depends on the coarseness of the model
elements.

BASIC OPERATION
1. Select the parent part

2. Click the Clip Icon

4. Position the Box Tool as desired.

3. Select Box Tool

5. Click Create

SEE ALSO
Introduction to Part Creation
How To Use Box Tool
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create IJK Clips
How to Create XYZ Clips
How to Create RTZ Clips.
User Manual: Clip Create/Update

Page 222

Create Quadric Clips

INTRODUCTION
In addition to standard clipping planes, EnSight also provides clipping against quadric shapes. These clips use the
corresponding quadric tool Cylinder, Sphere, Cone, Surface of Revolution) to specify the location of the clip.
As with clip planes, these tools can also be used to perform cut operations, creating parts which are the “inside” or
“outside” of the parent domain.
As with intersection clip planes, quadric clips can be changed interactively by manipulating the corresponding tool
with the mouse.

BASIC OPERATION
2. Click the Clip icon.

1. Select the parent part.

3. Select the desired quadric tool from the
Use Tool pulldown.
4. Select Finite or Infinite clip extents

6. Click Create.

5. Position the tool as desired (see the How
to for the applicable tool).

ADVANCED USAGE
Like the other clipping tools in EnSight, intersection quadric clips (except those created with the revolution tool) can
be interactive: as you drag the applicable tool with the mouse, the clip is automatically recalculated and redisplayed.
To perform interactive quadric clips:
1. Double-click the desired
quadric clip part in the
parts list.
2. Toggle on Interactive
Tool in the Quick
Interaction area.
3. Move the mouse into the
Graphics Window. Click on one of
the tool hotpoints (see the How to for
the applicable tool) and drag the tool
to the desired location.

Page 223

Cutting with Quadric Tools
A quadric tool can be used to create parts which are the result of a cut of its parent domain into “inside” and or
“outside” parts. These parts contain valid elements of the same order as the original domain parts.
1. Select the desired parent
parts in the parts list.
2. Click the Clip feature icon.
3. Select the desired Quadric
Tool.
4. Set the Domain to Inside,
Outside, or In/Out (both
inside and outside).
5. Hit the Create button.

Crinkly Quadric Clips
You can check the integrity of your mesh by clipping with a crinkly intersection. Specifying a Crinkly Domain results in
a part composed of all the elements of the mesh that intersect the quadric tool.

4. Change the Domain to
Crinkly.
5. Click the Apply Tool Change
button.

SEE ALSO
Introduction to Part Creation
How To Use the {Cylinder, Sphere, Cone, Surface of Revolution} Tool.
Other clips:
How to Create Clip Planes
How to Create Clip Lines
How to Create IJK Clips
How to Create XYZ Clips
How to Create RTZ Clips
How to Create Box Clips.
User Manual: Clip Create/Update

Page 224

Create IJK Clips

INTRODUCTION
An IJK clip is a 1D or 2D slice through a structured mesh. The resulting clip is a 1D line or 2D surface where one
dimension (e.g. I) is held fixed while the other one or two dimensions (e.g. J and K) vary. The minimum and
maximum range of the free dimensions can be set by the user, as well as the step size. IJK clips can be animated
throughout the range of the fixed dimension by manipulating a slider.
Although planar clips can still be created through structured meshes, it is often preferable to create IJK clips since
they are faster to calculate and use less memory. In addition, IJK clips are often more intuitive for the user (who
typically built the mesh).

BASIC OPERATION

1. Select the parent part.
2. Click the Clip icon.
3. Select IJK from the Use Tool pulldown.
4. Select the desired fixed dimension from the
Mesh Slice pulldown.

6. If you desire to modify values for the Min,
Max, and Step for the two free
dimensions, click this and the dialog
below will open up.
7. Click Create.

5. Enter the value for the fixed dimension in
the Value text field and press return.

Note that you can change the fixed dimension of an IJK clip at any time (with the Mesh Slice pulldown). If you change
one of the numeric values, remember to press return for the change to take effect.

Page 225

ADVANCED USAGE
Interactive IJK Clipping
You can interactively sweep through the range of the fixed dimension by adjusting a slider with the mouse.
1. Double-click the desired IJK clip part
in the parts list.
2. Change Interactive to Manual, to
enable sweeping.
3. Adjust the slider with the mouse.

Changing IJK Step Refinement
You can modify block-structured model parts to any level of IJK step refinement with proper updating of all dependent
parts and variables.
1. Select Edit > Part Feature Detail
Editors > Model Parts ... to open the
Feature Detail Editor (Model) dialog.

2. Select the structured part (or parts).

3. In the Creation Attributes area, enter
values into the From, To, and Step
fields based on their Min and Max
limits to update the refinement of the
respective I, J, and/or K mesh
component directions (remember to
press Return).

Clipping Plane Animation
Although you can interactively sweep an IJK clip through a mesh, it is sometimes desirable to have EnSight
automatically calculate a series of IJK clips for you. These can then be replayed (as fast as your graphics hardware
will permit) using EnSight’s Flipbook Animation facility. See How To Create a Flipbook Animation for more
information.

Page 226

SEE ALSO
Introduction to Part Creation
How To Create a Flipbook Animation.
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create XYZ Clips
How to Create RTZ Clips
How to Create Box Clips.
User Manual: Clip Create/Update

Page 227

Create XYZ Clips

INTRODUCTION
An XYZ clip is a 1D or 2D slice through 2D or 3D meshes (structured or unstructured). The resulting clip is a 1D or
2D mesh slice where one of the dimensions (e.g. X) is held constant (or fixed) while the other one or two dimensions
(e.g. Y and Z) vary in reference to the local frame of the mesh. XYZ clips can be interactively animated throughout
the range of the fixed dimension by manipulating a slider. The minimum, maximum, and step size of the range of the
interactive fixed dimension can be set by the user.

BASIC OPERATION

1. Select the parent part.
2. Click the Clip icon.

6. Click Create.

3. Select XYZ from the Use Tool pulldown.
4. Select the desired fixed dimension from the
Mesh Slice pulldown.
5. Enter the value for the fixed dimension in
the Value text field and press return.
Note: Multiple slices with a delta in the normal direction can be created easily by setting these values.

Note that you can change the fixed dimension of an XYZ clip at any time (with the Mesh Slice pulldown). If you
change the numeric value, remember to press return for the change to take effect.

Shortcut
In Part Mode, right click on a part in the graphics window. In the resulting pulldown, choose Clip and in the further
pulldown, choose X, Y, or Z. This then automatically creates an X, Y, or Z clip part with the default settings using the
right-clicked part as the parent part.

Page 228

ADVANCED USAGE
Interactive XYZ Clipping
You can interactively sweep through the range of the fixed dimension by adjusting a slider with the mouse.
1. Double-click the desired XYZ clip
part in the main parts list.
2. Change Interactive to Manual to
enable sweeping.
3. If desired, enter values for the Min,
Max, and Increment to override the
defaults (remember to press return).
4. Adjust the slider with the mouse.

Crinkly XYZ Clipping
You can check the integrity of your mesh by clipping with a crinkly intersection. Specifying a crinkly domain results in
a part composed of all the elements that intersect the mesh slice value.
1. Change the Domain to Crinkly

Clipping Plane Animation
Although you can interactively sweep an XYZ clip through a mesh, it is sometimes desirable to have EnSight
automatically calculate a series of XYZ clips for you. These can then be replayed (as fast as your graphics hardware
will permit) using EnSight’s Flipbook Animation facility. See How To Create a Flipbook Animation for more
information.

SEE ALSO
Introduction to Part Creation
How To Create a Flipbook Animation
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create IJK Clips
How to Create RTZ Clips
How to Create Box Clips.
User Manual: Clip Create/Update

Page 229

Create RTZ Clips

INTRODUCTION
An RTZ clip is a 1D or 2D slice through 2D or 3D meshes (structured or unstructured). The resulting clip is a 1D or 2D
mesh slice where one of the dimensions (e.g. R,”radial component”) is held constant (or fixed) while the other one or
two dimensions (e.g. T, ”theta component” and Z, “z axis component”) vary in reference to the local frame of the
mesh. RTZ clips can be interactively animated throughout the range of the fixed dimension by manipulating a slider.
The minimum, maximum, and step size of the range of the interactive fixed dimension can be set by the user.

BASIC OPERATION

1. Select the parent part.
2. Click the Clip icon.

7. Click Create.

3. Select RTZ from the Use Tool pulldown
4. Select the Axis that describes the
cylindrical length.
5. Select the desired fixed dimension of the
slice (R, T, or Z).
6. Enter the value for the slice (the value of
R, T, or Z), and press return.
Note that you can change the fixed dimension of an RTZ clip at any time (with the Slice pulldown). If you change the
numeric value, remember to press return for the change to take effect.

ADVANCED USAGE
Interactive RTZ Clipping
You can interactively sweep through the range of the fixed dimension by adjusting a slider with the mouse.
1. Double-click the desired RTZ clip
part in the main parts list.
2. Change Interactive to Manual to
enable sweeping.
3. If desired, enter values for the Min,
Max, and Increment to override the
defaults (remember to press return).
4. Adjust the slider with the mouse.

Page 230

Crinkly RTZ Clipping
You can check the integrity of your mesh by clipping with a crinkly intersection. Specifying a crinkly domain results in
a part composed of all the elements that intersect the mesh slice value. Crinkly clipping cannot be done interactively.
1. Change the Domain to Crinkly

Clipping Plane Animation
Although you can interactively sweep an RTZ clip through a mesh, it is sometimes desirable to have EnSight
automatically calculate a series of RTZ clips for you. These can then be replayed (as fast as your graphics hardware
will permit) using EnSight’s Flipbook Animation facility. See How To Create a Flipbook Animation for more
information.

OTHER NOTES
Inside, Outside, and In/Out cutting are disabled for this clipping type because it has no meaning for T. And if you
desire this effect for Z or R, you can use a plane clip or cylindrical clip instead.

SEE ALSO
Introduction to Part Creation
How To Create a Flipbook Animation
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create IJK Clips
How to Create XYZ Clips
How to Create Box Clips.
User Manual: Clip Create/Update

Page 231

Create Revolution Tool Clips

INTRODUCTION
A Revolution Tool clip can be made using the surface of revolution tool. It can be the surface created by the
intersection of the surface of revolution tool and the model, the elements intersected by the surface of revolution tool
(crinkly), or the volume of the inside and/or the outside domain swept by the revolution tool. This clip does not have
interactive manipulation capability, with a slider or by dragging the tool with the mouse. However, the tool can be
manipulated and the clip updated.

BASIC OPERATION

1. Place the Surface of Revolution Tool at the
desired location. See How To Use the
Surface of Revolution Tool.
2. Select the parent part.
3. Click the Clip icon.
4. Select Revolution Tool from the Use Tool
pulldown.
5. Select the desired Domain.
6. Select extents

7. Click Create.

Note that you can manipulate the Surface
of Revolution tool and update your clip by
and clicking Apply Tool Change.
You can also change the domain, and the
clip will change.

ADVANCED USAGE
SEE ALSO
Introduction to Part Creation
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create XYZ Clips
How to Create RTZ Clips
How to Create Box Clips
How to Create IJK Clips
How to Create Revolution of 1D Part Clips.
User Manual: Clip Create/Update

Page 232

Create Revolution of 1D Part Clips

INTRODUCTION
A Revolution of 1D Part clip can be made using a 1D part and a user specified axis. It can be the surface created by
the intersection of the 1D part about the axis and the model, the elements intersected by the 1D part about the
axis(crinkly), or the volume of the inside and/or the outside domain swept by the 1D part about the axis. This clip does
not have interactive manipulation capability, with a slider or by dragging the tool with the mouse. However, if the 1D
part is capable of being moved, you can move it and the revolution clip will update.

BASIC OPERATION

1. Select the parent part.

6. Click Create.

2. Click the Clip Icon.
3. Select Revolve 1D Part from the Use Tool
pulldown.
4. Enter the 1D part to use.
5. Set the desired origin and axis of the
revolution.
6. Select the desired Domain.

Note that you can manipulate the 1D part
or the origin and axis and the clip will
update.
You can also change the domain, and the
clip will change.

ADVANCED USAGE
SEE ALSO
Introduction to Part Creation
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create XYZ Clips
How to Create RTZ Clips
How to Create Box Clips
How to Create IJK Clips
How to Create Revolution Tool Clips.
User Manual: Clip Create/Update

Page 233

Create General Quadric Clips

INTRODUCTION
Double Clicking on the Clip Create/Update Icon brings up the Feature Detail Editor (Clips), the Creation attributes
section of which offers access to one type of clip creation which is not available in the Quick Interaction area. It is
possible to create a 3D Quadric clip using the General Quadric option by directly specifying the coefficients of a
general quadric equation.
These coefficient values represent the general equation of a Quadric surface. They can be changed by modifying the
coefficient values. No tool exists corresponding to this equation.
AX2+BY2+CZ2+DXY+EYZ+FXZ+GX+HY+IZ=J

BASIC OPERATION
1. Get to the Feature Detail Editor for clips.
The easiest way to do this is to double click
the Clip Feature Icon.
2. Select the parent part(s) in the Parts list.

3. Choose the General Quadric Tool.
4. Choose the desired Domain (Intersect,
Crinkly, Inside, Outside, or In/Out)
5. Edit the coefficients.
3. Click the Create button.

Note: The Animation Delta is not available for
general quadric clips.

Page 234

SEE ALSO
Introduction to Part Creation
Other clips:
How to Create Clip Lines
How to Create Clip Planes
How to Create Quadric Clips
How to Create XYZ Clips
How to Create RTZ Clips
How to Create Box Clips
How to Create IJK Clips
How to Create Revolution Tool Clips.
User Manual: Clip Create/Update

Page 235

Create Clip Splines

INTRODUCTION
In addition to clipping along a line, EnSight also provides clipping along a defined spline. Spline clips will query the 2D
or 3D parent parts at samples taken along the spline at evenly spaced intervals. Values along a spline clip can be
visualized using profiles, queried and sent to a plotter, or used in further computations (for example a line integral).

BASIC OPERATION
2. Click the Clip icon.

1. Select the parent part.

3. Select Spline from the Use Tool pull-down.
4. Select the desired Spline (to create a
Spline see How To Use the Spline Tool)
5. Set the number of evenly spaced points
on the line

6. Click Create.

Note: To adjust the clip you can grab the spline knot points and adjust. The clip will update.

Page 236

OTHER NOTES
It is sometimes useful to display just the nodes of a spline clip. Using the Feature Detail Editor you can change the
display such that only nodes (not lines) are displayed. The nodes can be shown as dots, crosses, or spheres. If
displayed as crosses or spheres, the size (radius) can be contant or scaled by the value of a variable. See How to
Set Attributes for more information.

SEE ALSO
Introduction to Part Creation
How To Use the Spline Tool
How to Create Profile Plots
How to Query/Plot.
Other clips:
How to Create Clip Planes
How to Create Clip Lines
How to Create Quadric Clips
How to Create Box Clips
How to Create IJK Clips
How to Create XYZ Clips
How to Create RTZ Clips.
User Manual: Clip Create/Update

Page 237

Create Vector Arrows

INTRODUCTION
Vector arrows display the direction and magnitude of a vector at discrete locations in a model. Although vector
magnitude can be visualized with other methods (e.g. color), important directional information is provided by the
arrows.
Vector arrows have numerous attributes including length scale, tip style and size, projection, origin location, and
display filters based on vector magnitude.

BASIC OPERATION
2. Click the Vector Arrows icon.

1. Select the parent.
part.

3. Select the vector variable to use.
4. Click Get Default to load a suitable Scale Factor.
5. Click “Create”.

Arrow Tips
To change the arrow tip shape, click the Arrow Tips button to open the Vector Arrow Tip Settings dialog:
Tip Shape Choices:

1. Select the desired tip shape from the
Shape pulldown (see description at right).
2. Select a color (for Tipped shape only).
3. From the Size pulldown, select whether tip
scaling is Fixed (and enter an appropriate
value in the text field) or Proportional to the
local vector magnitude.

None

No tip (default).

Cone

Solid cone shape

Normal

Single wedge. Good for 2D
problems. Plane of the
wedge is based on the
relative magnitudes of the
components.

Triangles

Two intersecting triangles.
Good for 2D/3D problems.

Tipped

End of the shaft colored in a
different color. Good where
other shapes yield too much
visual clutter.

Page 238

Other Vector Arrow Attributes
Other vector arrow attributes control the type of arrow, the location of the arrow origin, and arrow filtering options
based on vector magnitude:
1. Double-click the desired vector arrow part in the parts list.
2. Select the desired type from the Type pulldown.
Choices are:
Rectilinear

Standard vector arrows: shaft points in local vector direction with
length equal to vector magnitude scaled by Scale Factor Value.

Rect. Fixed

Same as Rectilinear except that length is set by Scale Factor value
independent of vector magnitude.

Curved

Arrow shaft is the path of a particle trace in the local flow field. Scale
Factor becomes “Time” and controls the duration (stopping criteria)
for each trace. WARNING! This can take a great deal of time for
large numbers of vector arrows and/or long Time values!

3. Select the desired filter type from the Filter
pulldown.

5. Select the desired arrow origin from the
Location pulldown.

Choices are:

Choices are:

None

No filtering – all vector arrows appear.

Node

Low

Display only those arrows with magnitude
above the value in the Low text field.

Arrows originate from each node of the parent
part(s).

Vertices

Display only those arrows with magnitude
below Low and above High (opposite of Low/
High).

Arrows originate only from those nodes that
are also vertices of the parent part(s).

Element Center Arrows originate from the geometric center
of all elements of the parent part(s).

Band

High

Display only those arrows with magnitude
below the value in the High text field.

Low/High

Display only those arrows with magnitude
between Low and High (opposite of Band).

4. Select the desired density (0.0 to 1.0).
A density of the arrows will vary from no arrows (0.0) to
arrows at every location (1.0). At intermediate densities
the arrows are placed randomly.

Shortcut
In Part Mode, right click on a part in the graphics window. In the resulting pulldown, choose Vector Arrows. A window
will pop up to choose a variable if there are more than one vector variables. This then automatically creates an vector
arrow part with the default settings using the selected vector variable (or if only one using that one) and using the
right-clicked part as the parent part.

Page 239

ADVANCED USAGE
Although not accessible from the Vector Arrows Quick Interaction area, you can also change the projection of vector
arrows and the display offset.
1. Open the Feature Detail Editor for Vector
Arrows (Edit > Part Detail Editors... > Vector
Arrows).
2. Select the desired vector arrow part.

3. Select the desired projection type from the
Projection pulldown.
The projection choices are modified by the settings
in the Projection components X,Y,Z numeric fields.
These values represent a scaling factor for the
component. Zero means that the component
should not be considered (and therefore confine the
arrows to the plane perpendicular to that axis). One
is the default setting; values less than 1 diminish the
contribution of the component while values greater
than 1 exaggerate the contribution.
Choices for Projection are:
All

Display arrows based on the vector direction
as modified by the Projection Component
values.

Normal

Display arrows based on the “All” vector but
in the direction of the surface normal at the
arrow origin.

Tangential

Display arrows based on the “All” vector but
projected tangential to the surface at the
arrow origin. This is good for locating flow
components perpendicular to the main flow
direction (such as vortices).

Component

Display both the Normal and the Tangential
arrows.

4. Set the desired display offset.
The display offset is used to displace the vector arrows a
short distance away from the surface on which they are
defined (typically for hardcopy or animation purposes). This
is typically necessary when a tangential projection is used
and the arrows are coincident with the parent part’s surface.
Note that a negative offset may be appropriate (depending on
orientation).

OTHER NOTES
Vector arrows can be animated by animating the parent part (e.g. a clip plane) over space or time using flipbook or
keyframe animation. See How To Create a Flipbook Animation or How to Create a Keyframe Animation for
more information.
If vector arrows are created on a clip through an unstructured mesh, the resulting arrows can be difficult to visualize if
the resolution of the underlying mesh varies substantially or is highly irregular. One solution is to create the vector
arrows on a grid clip rather than the default mesh clip. See How to Create Clip Planes for more information.

Page 240

Unlike most part creation operators, vector arrows are created from the client’s representation of the part – not the
server’s. For example, if you have a clip plane that is displayed using a feature-angle or border representation, only
those elements comprising the reduced display will yield vector arrows – even though all elements of the clip plane
reside on the server. See How to Change Visual Representation for more information.
Vector arrows with a tangential projection can sometimes by occluded by the surface on which the arrows are
defined. To solve this problem, use the Display Offset field to add a small displacement to move the arrows away
from the surface. This is most useful for presentation (e.g. hardcopy or animation) output.

SEE ALSO
Introduction to Part Creation.
User Manual: Vector Arrow Create/Update

Page 241

Page 242

Create Elevated Surfaces

INTRODUCTION
An Elevated Surface is a 2D surface scaled (in the local surface normal direction of the parent) based on a variable
value. Elevated surfaces resemble topographic maps and are useful for accentuating relative differences in the value
of a variable. An Offset Surface uses a rigid-body translated origin part translated within a 3D parent part, to create a
new part using the geometry of the origin part, while getting variable information from the parent part. In other words,
an Offset Part results from using a translated orgin part to clip a 3D volume parent part.

BASIC OPERATION
Elevated Surface

1. Select the parent part.
3. Select ‘Elevated’.
4. Select the variable to use.

2. Click the elevated surface creation icon.

5. Select an appropriate scale factor
(or click the Get Default button).
6. If desired, enter an Offset value and press return.
The Offset allows you to “shift” the elevated surface
away from the parent, but does not affect the shape.
7. If desired, toggle Surface or Sidewalls off.
The Surface is the actual elevated surface. You can
also have Sidewalls which stretch from the border of
the parent to the border of the Surface to enclose the
created part.

Offset Surface

8. Click “Create”.

1. Select the 3D parent part
(see item 1 above).
2. Click the elevated surface icon
(see item 2 above).
3. Select ‘Offset’.
4. Choose the translation vector direction
and scale. The rigid-body translation is
equal to offset_scale * offset_vector
5. Choose the origin part which will be
used to clip the parent part at a location
specified by the rigid-body translation.

6. Click “Create”

SEE ALSO
User Manual: Elevated/Offset Surface Create/Update

Page 243

Extrude Parts

INTRODUCTION
A part or parts can be “extruded” to the next higher ordered part using the Extrusion feature. Namely, a 1d line can
become a plane, a 2D surface can become a volume, etc. This “extrusion” can occur in a rotational way (making the
whole pie from a thin slice) such as would be needed for reconstruction of a model from an axi-symmetric slice. Or it
can be done in a translational manner - as if the part were glued in place, but could be stretched in one direction.
For rotation extrusions, you must define an origin and axis vector in the global coordinate system, about which the
rotational extrusion will occur, as well as the number of slices and the total rotation angle to sweep through. For
translation extrusions, you define a direction vector in the global coordinate system, as well as the number of slices
and the total distance to stretch.

BASIC OPERATION
Rotational Extrusion:
1. Select the parent part.

2. Click the Extrusion icon.

3. Select Rotation type
4. Set the number of “slices” that will be created.
5. Set the total rotation to extrude.
(Needs to be between -360 and 360)
6. Set the origin of the rotation axis
8. Click Create.

7. Set the components (direction cosines)of the
rotation general axis.

This will cause a 2D slice to become a 3D volume.

Page 244

Translational Extrusion:

1. and 2. as above
3. Select Translation type.
4. Set the number of slices in the translation
direction.
5. Set the total translation distance.
6. Set the components of the direction vector.
7. Hit Create.

And the slice will now become something like the
following:

SEE ALSO
User Manual: Extrusion Parts Create/Update

Page 245

Create Profile Plots

INTRODUCTION
A profile plot is the 2D counterpart to an elevated surface: a projection away from a 1D part based on the value of a
variable. Profile plots can be created on any 1D part: clip lines, contours, particle traces, or model parts consisting
of 1D elements.

BASIC OPERATION
2. Click the profile creation icon.

1. Select the parent part.
3. Select the variable to use.

4. Select an appropriate Scale Factor (or click
Get Default).
5. If desired, enter an Offset value and press return.
The Offset allows you to “shift” the profile away from the
parent, but does not effect the shape.
6. If desired, adjust the orientation of the Plane tool.
The Plane Tool is used to specify the orientation and
direction of the profile plot. See below for more
information.

7. Click “Create”.

For each node of the parent part, the corresponding node on the profile curve is determined by adding the value of
the Offset to the selected variable and then multiplying the sum by the Scale Factor. The projectors of the profile are
the lines that connect the nodes of the parent part to the nodes of the profile curve. The Plane tool is used to specify
the orientation and direction of the projectors. The projectors are created parallel to the Plane tool projecting away
from the center of the Plane tool (at least where the value of the selected variable plus the Offset is positive).
Although the parent part of a profile plot must be 1D, the nodes that make up the part do not have to be linear. For
curved parents, the projectors of the resulting profile plot are still parallel, but they do not all lie in the same plane.

SEE ALSO
User Manual: Profile Create/Update

Page 246

Create Developed (Unrolled) Surfaces

INTRODUCTION
EnSight provides several sophisticated tools for extracting computational surfaces from meshes. For model parts or
clipped surfaces with a defined axis of rotation (such as those created with the quadric clipping tools), the surface can
“developed” or unrolled onto a plane. All variables defined on the clip are properly interpolated onto to the developed
surface.
A clip can be developed based on curvilinear (radius, z), (theta, z), or (meridian, theta) coordinate projections. The
“seam” of the clip can be specified interactively.
A model part must have its seam, its longitudinal axis and origin defined appropriately in the Feature Detailed Editor
(developed surface settings). To do this, right click on the part, choose ‘Edit’ and then pick the developed surface
icon in the top of the window that pops up and define the entities appropriately.

BASIC OPERATION
To create a developed surface:
1. First, create the desired quadric clip (cylinder, sphere, or cone), or
skip this step if your quadric model part already exists.
3. Click the Developed
Surface icon.
4. Select the desired projection type (see
below for details on the types).

2. Select the parent part for the
developed surface (i.e. the part
you created in step 1).

5. If applicable for the projection type (and desired)
enter u,v scaling factors and press return).
6. To display and change the cutting seam, click the
Show Cutting Seam button, and adjust the slider.
7. Click Create.

A part is developed by specifying one of three curvilinear mappings called developed projections. The projections are
based on the curvilinear coordinates r (radius), z, θ (theta), and m (meridian or longitude). These coordinates are
defined relative to the local origin and axis of the tool that created the parent part (e.g. the Cylinder tool). The
projections are (r,z), (θ, z), and (m, θ). The u, v scale factors (only for (θ, z) or (m, θ) projections) provide scaling for
the coordinates in the listed order. For example, if the projection is (θ, z) then u scales θ and v scales z.

SEE ALSO
How To Create Quadric Clips
User Manual: Developed Surface Create/Update

Page 247

Create Subset Parts

INTRODUCTION
A Subset Part can be created by specifying node and/or element label ranges of a model part. Subset Parts can only
be created from model parts that have node and/or element labels. The Subset Part feature can be used to isolate
specified nodal and element regions of interest in large data sets.

BASIC OPERATION
1. First, click the Subset Parts creation icon.

3. Select Elements (or Nodes) to Show.

2. Now, for each parent model part,
enter the part number of the
desired parent part in the Add field
and press return.

4. Enter the element (or node) label range(s) in
the Show List text field (ranges are separated
by commas).
OR
Toggle on “Pick elements” and select
elements using pick selection, which by
default is the “p” keyboard key.
OR
Turn on the selection tool and place it where
desired, then click “Add elements from
selection tool” to pick all the elements within
the tool.
5. Click Create

SEE ALSO
How To Probe Interactively
User Manual: Subset Parts Create/Update

Page 248

Create Tensor Glyphs

INTRODUCTION
Tensor glyphs display the direction of the eigenvectors for a tensor variable. Controls exist to show just the
compressive or tensile eigenvectors, and to selectively show the minor, middle, or major vectors.
Tensor glyphs have numerous attributes including length scale, tips, color, and line width which can be used to
indicate compression or tension.

BASIC OPERATION
3. Select the tensor
variable to use.

2. Click the Tensor Glyph icon (by default this icon is
not displayed unless you have enabled it through
Edit > Preferences > General User Interface
“Modify and save icon layout”).

1. Select the parent
parts.

4. Select which
eigenvectors to display.

5. Click Create.

Display Attributes
The glyph’s attributes to indicate tension or compression can be modified in several ways. Click the Display
Attributes button to open the Tensor Display Attributes dialog:
1. Select the desired tip shape from the Tip Shape pulldown.
Tip Shape Choices:
None

No tip (default)

Normal

Single wedge. Good for 2D problems.
Plane of the wedge is based on the
relative magnitudes of the components.

Triangles

Two intersecting triangles. Good for 2D/
3D problems.

2. The glyph can either be colored by
the part color, or show a specified
color for compressions and tension.
3. The glyph can either be shown with the line width attribute of the glyph,
or show a different line width for tension and compression.

Page 249

OTHER NOTES
Tensor glyphs can be animated by animating the parent part (e.g. a clip plane) over space or time using flipbook or
keyframe animation. See How To Create Flipbook Animation or How to Create a Keyframe Animation for more
information.
Unlike most part creation operators, tensor glyphs are created from the client’s representation of the part - not the
server’s. For example, if you have a clip plane that is displayed using a feature angle or border representation, only
those elements comprising the reduced display will yield tensor glyphs - even though all elements of the clip plane
reside on the server. See How to Change Visual Representation for more information.

SEE ALSO
Introduction to Part Creation.
User Manual: Tensor Glyph Parts Create/Update

Page 250

Display Displacements

INTRODUCTION
In structural mechanics simulations, a common output variable is a set of vectors representing the movement or
displacement of geometry. Each displacement vector specifies a translation of a node from its original position (an
offset). EnSight can display and animate these displacements to help visualize the relative motion of geometry.
In many cases, the magnitude of the actual displacements is extremely small relative to the size of the model.
EnSight provides a displacement factor to scale the vectors and exaggerate the displacement.
Normally, displacements are applied in the EnSight Client - providing the proper visual modifications needed.
However, EnSight can actually modify the geometry on the server according to a model displacement variable (not
computed variables). Server side applied displacements will yield proper volumes and other computed attributes.

BASIC OPERATION

1. Select the parent parts.
2. Click the Part tab.

3. Click the displacement
creation icon.

4. Select the nodal variable to
use. Limitation: can only
use nodal vector variables.
5. If desired, enter a value for the
Displacement Factor and press
return.
6. For speed and memory, default is
visual displacement only. If you
desire to use the displacement in
any calculations then toggle on
server-side displacements.
Note that your changes in the Quick Interaction area are immediate. Specifying a displacement does not create a
new part, it merely sets the displacement attributes for the selected parts.
Page 251

Server Side Displacements
Server side displacements have more detailed
attributes found in the Part Feature Detail Editor.
1. First read in your model, build the desired parts,
and activate the model variable (not computed
variables) representing displacement.
2. Open the Feature Detail Editor (Model).
Use Edit > Part feature detail editors > Model parts, or
just right click on the partlist and choose ‘Edit’
3. Select the desired parts.
4. Set the desired scale factor for the displacement.
Hit a carriage return.
5. Set the nodal displacement model variable and
the translation for each component.
Hit a carriage return.
6. Hit the Apply changes button.
Note that it is possible displace in each component
direction by a different variable and to translate by a
single value in each direction. It is also possible to
scale the entire geometry by a factor. Enter in a nodal
vector variable and the correct component will be
extracted.

Displacement applied in this manner actually modifies
the geometry on the server (not just the visual
representation on the client). Any queries or
computations will reflect this modified geometry. For
example area or volume calculation will now use the
displaced values.

Page 252

ADVANCED USAGE
Vibrational analysis typically produces eigenvectors. EnSight can animate these vectors as mode shapes to
visualize selected vibration modes (each represented by a different displacement vector). The EnSight Flipbook is
used to build and load the animation. Once loaded, the animation can be replayed while still providing viewing
control. To create a mode shape flipbook:
1. Be sure displacements are active
and the Displacement Factor is set
to a suitable value (as described
above).
2. Click the Flipbook icon.

3. Select Mode Shapes from
the Load Type pulldown.

4. Enter the desired number of
Flipbook pages to create.
5. Click “Load”.
6. Once loading is complete it will
automatically change to the Run
tab and the animation will be
running.

The first page of the animation shows the full displacement (as it is shown in the Graphics Window without the
Flipbook) while the last page shows full displacement in the opposite direction. Intermediate pages show
displacements as driven by the cosine function.
Note that you can create copies or extracts of parts and simultaneously display them with different mode shape
variables or to show the initial static state along with the mode shape animation.

SEE ALSO
See How To Create a Flipbook Animation for more information on Flipbooks.
User Manual: Part Displacement, Flipbook Animation

Page 253

Display Discrete or Experimental Data

INTRODUCTION
In addition to meshed data consisting of nodes and elements, EnSight also supports discrete or measured data. A
measured dataset consists of a series of arbitrary points in space with no connectivity. Measured data can have
associated variable data and can vary over time. Examples of measured data include fuel sprays, multi-phase flows,
and experimental data.
Measured data cannot be loaded by itself – you must also specify a regular geometric mesh.

BASIC OPERATION
Measured data is read into EnSight via the same dialog used to read meshed data:
1. Select File > Data (Reader)... to open the File Selection dialog for data file selection.

2. Find the directory containing the
data (see How To Read Data for
more information on using File
Selection).
3. If desired, select and specify a
(meshed) geometry file and the
corresponding result file.
4. Select the measured result file in
the Files list.

5. If desired, specify an initial time
step (the last step is the default).

6. If you are reading a meshed
dataset (as directed in step 3),
select the file format.

7. Click (Set) Measured to specify
the selected measured result file.

8. Click Okay to begin the reading
process.

9. The Data Part Loader dialog
corresponding to the selected data file
format (as set in step 6) will open. You do not have to perform any further action to load the
measured data. However, if you are also loading meshed data, continue with the usual part loading
process. For details, see the How To article for the chosen file format.

Page 254

Measured data is represented as a single part. In the Main Parts list you should see a part named “Measured/
Particle” after loading.
Measured data is represented as a set of unconnected nodes. You can use EnSight’s ability to display nodes in
various ways to accentuate measured data visualization. To change node display:
1. Select the desired measured data part in the
Main Parts list.
2. Click Part in the Mode Selection area to enter
Part Mode.
3. Click the Node Representation icon to open
the Part Node Representation dialog.

4. Select the desired node display type (Dot,
Cross, or Sphere). See below for details on
each type.
5. If applicable, set desired values for Scale,
Detail, Size By, and Variable.
• Dot: nodes are displayed as points.
• Cross: nodes are displayed as crosses and can be
fixed size (size set by the Scale value) or sized
based on a Variable (and scaled by the Scale
value).
• Sphere: nodes are displayed as spheres and can
be fixed size (size set by the Scale value) or sized
based on a Variable (and scaled by the Scale
value). Sphere detail controlled by Detail value.

OTHER NOTES
The file formats for measured data and the measured results file are detailed in EnSight5 Measured/Particle File
Format.
Transient measured data can be animated using either the flipbook or keyframe animation capability.
You can load multiple measured datasets simultaneously by using EnSight’s cases capability.

SEE ALSO
User Manual: EnSight5 Measured/Particle File Format

Page 255

Change Time Steps

INTRODUCTION
From it’s inception, EnSight has been used extensively to postprocess time-varying or transient data. In many cases,
dynamic phenomena can only be understood through interactive exploration. The Solution Time Quick Interaction
area provides the interface for working with transient data and provides comprehensive control over time handling.

BASIC OPERATION
EnSight provides two ways to work with transient data. By default, time is presented as a series of discrete steps
running from zero to the total number of steps minus one. However, you can also present time based on the actual
simulation time values found in your results data. The presentation mode is controlled by the Time As pulldown
menu. In the dialog below, Time As is set to Step and time is presented as discrete steps running from 0 to 159 (160
total steps). The simulation time (as reported in the top line of the dialog) runs from 1.0 to 160.0.
The current time range is displayed in the Beg and End fields with the current time step shown in the Cur field. You
can modify the time range displayed in the slider by editing the Beg and/or End fields (remember to press return).
You can change the current time step by editing the Cur field (press return), manipulating the slider, or clicking the
left/right slider arrows. Clicking Reset Time Range will reset Beg and End to the full range.
Time scaling and stepping (as manipulated through the slider bar and Beg, Cur, and End fields) can either be
Discrete or Continuous. If scaling is Discrete, only your actual time steps as written in the results data can be
visualized. In addition, the Beg, Cur, and End fields can only be set to integer values (if Time As is set to Step and
Scale Type is Discrete) or actual simulation times represented in your results data (if Time As is set to Sim. Time). If
scaling is Continuous, you can display results between your actual output time steps (all variable values are linearly
interpolated between the two surrounding time steps). Note that if your mesh is changing over time (either set of
elements or element connectivity) you cannot display results continuously.
When you manipulate the slider or change the Cur field, EnSight will perform all tasks necessary to correctly display
the new time step in the Graphics Window. Depending on the size of the dataset and the number of additional parts
you have created, this may take a significant amount of time. If you wish to create an on-screen animation of your
results, use the Flipbook facility (click Animate Over Time to quickly jump to the Flipbook Quick Interaction area).
To use the Solution Time Quick Interaction area:
1. Click the Solution Time icon in the Feature
Icon bar.
2. Make changes as desired.

The Beg and End fields control the available
time range (and also the range of the slider
action). The range markers on the slider can
be moved to set these values or you can
enter new values into the fields and press
return.
The Current field sets the current time step.
Either move the center slider or enter a new
value in the field and press return.

The slider bar lets you step through time. Grab the slider and dial to
the desired time or click the left/right slider arrows to increment (the
increment can be set by changing the Increment field).

Click to display time as annotation in the
graphics window.
Click to open the Flipbook Animation Quick
Interaction area.
Set Scale Type to Discrete or Continuous
(see above for details).

Set the number of time cycles in
the time range.

Set Units to Step or Sim. Time
(see above for details).

Set the step increment size for the
slider arrows. Must be an integer
if Scale Type is Discrete.

Page 256

Recording an Animation of your data:
You can stream data from disk by using
the VCR type controls. Namely, hit the
Play button.

While this is occurring, the Record button will be brightly colored red and
can be clicked to record the animation that is occurring.
Note: This is similar to a flipbook animation loaded as images, but does not
require additional workstation memory. Thus, it is a simple way to record an
animation of your transient data.
This recording process is explained in How To Print/Save an Image

Page 257

ADVANCED USAGE
EnSight allows geometry and variables to behave in a transient manner on different timelines, i.e., a variable called
Temperature can be defined at t = 0., 3., and 6. while a variable called Pressure can be defined at t = 0., 2., and 5.5.
The Timeset Details button will bring up the Timeset Details dialog which allows the user to view the various timelines
as well as specify how the variables will behave when they are not defined.
The EnSight case file defines the timesets (name and associated time values) and associates a timeset with each of
the variables and geometry.
By default the Solution Time dialog will show a composite of all of the timesteps that exist across all of the timesets.
This can, however be changed to show just the time values associated with a particular timeset.
In the Timeset Details dialog shown below, multiple timesets exists. Three timesets (from the Which Timeset(s) list)
are selected and are thus shown in detail. The graphics for each timeset shows (a) the minimum and maximum
overall time value, (b) white tick marks immediately under the timeline indicate the total (composite) time values
available from the solution time dialog, (c) green tick marks indicating the time values defined for the timeset, (d) the
current time value (indicated with the long green line) associated with the timeset.

The current solution time (as
set in the Solution Time dialog.

To modify all the timelines to
behave the same way, select
which range is to be modified,
then select how they will be
displayed.

Select the timeline to be
viewed.

The timeset can either be
shown having a time range
over the total number of time
values or can be shown
according to the timeset’s
range.

By default the Solution
Time dialog shows the
composite timeline.
This button will modify
the Solution Time
dialog’s Beg and End
values to those of the
selected timeset.

Shows the time value being
used at the current time.
The timeset is used by the
variables (or geometry)
shown in this list.

When the current time (from the
Solution Time dialog and indicated
in the upper left corner of this
dialog) is set to a value less than
what is available for this timeline,
use the Nearest value or make the
variable Undefined.

When the current time (from the
Solution Time dialog and indicated
in the upper left corner of this
dialog) is set to a value that does
not exist for this timeline,
Interpolate between defined time
values, use the Left, Right, or
Nearest value, or make the
variable Undefined.

When the current time (from the
Solution Time dialog and indicated in
the upper left corner of this dialog) is
set to a value greater than what is
available for this timeline, use the
Nearest value or make the variable
Undefined.

SEE ALSO
How To Load Transient Data, How To Animate Transient Data
User Manual: Flipbook Animation

Page 258

Extract Vortex Cores

INTRODUCTION
Vortex cores are centers of swirling flow where the velocity is parallel to the vorticity. For a more complete description
refer to the User Manual section below.

BASIC OPERATION
1. Select the parent part.

2. Select the Vortex Core icon on the second row of icons.

3. Bring up the Vortex Core
Variable Settings dialog by
clicking here.

4. Define either (Density and
Momentum) or Velocity, as well
as the Ratio of Specific Heats.
The variables can be set by
either typing them into the
fields, or selecting them from
the list above and clicking the
Set button.

5. Click Okay to finish the
variable setup.
6. Click Create.

Page 259

ADVANCED USAGE
The resulting vortex core lines can be filtered by the vortex core strength or by any other active variable.

1. Select the variable to filter by.
2. Set the Threshold filter to remove the portion of
the vortex core that is larger or less than the
specified threshold value.
3. Enter a threshold value
- or 3. Slide the slider to a new threshold value.

OTHER NOTES
Extract Vortex Cores does not work with more than one case.

SEE ALSO
User Manual: Vortex Core Create/Update

Page 260

Extract Separation and Attachment Lines

INTRODUCTION
Separation and attachment lines are created on any 2D surface and show interfaces where flow abruptly leaves
(separates) or returns (attaches) to the surface. For a more complete description refer to the User Manual section
below.

BASIC OPERATION
1. Select the 2D parent part.
2. Click the Separation/Attachment part
icon.

3. Bring up the dialog
defining the necessary
variables by clicking here.

4. Define either Density and
Momentum or velocity, as
well as the Ratio of Specific
Heats.
The variables can be set by
either typing them into the
fields or be selecting them
from the list above and
clicking the Set button.

6. Click Create

5. Click Okay to finish the
variable setup.

This will create two parts one each for the separation
and attachment lines. You
can modify the visual
attributes of these parts
separately, but when you
change any creation
attribute, both parts will be
modified.

Page 261

ADVANCED USAGE
The resulting separation/attachment parts can be filtered by the fx_sep_att_strength variable or by any other active
variable.

1. Select the variable to filter by.
2. Set the Threshold filter to remove the portion of the
separation/attachment line that is larger or smaller than
the specified threshold value.
3. Enter a threshold value
- or 3. Slide the slider to a new threshold value.

OTHER NOTES
The separation and attachment parts are linked together with regard to their creation attributes, i.e. when one is
modified the other is also. Further, when one is deleted the other is also deleted.
Separation and Attachment feature extraction only works with one case.
The separation and attachment line parts should generally not interfere visually with the 2D parent parts they lie on
(as long as the preference for graphics hardware offset is on - see View Preferences), but they may interfere if
printed. In either case you can apply a display offset manually to avoid the interference in the Feature Detail Editor for
the part. The display offset will be in the direction of the parent surface normal.

SEE ALSO
User Manual: Separation/Attachment Lines Create/Update

Page 262

Extract Shock Surfaces

INTRODUCTION
Shock surfaces and regions help visualize shock waves in 3D (trans/super-sonic) flow. For a more complete
description, refer to the User Manual section below.

BASIC OPERATION
1. Select the parent part.
2. Click the Shock Surface/Region icon.

3. Bring up the dialog defining
the necessary variables by
clicking here.

4. Define either Density
or (Temperature and
Pressure), (Energy or
Pressure), (Momentum or
Velocity), and Ratio of
Specific Heats.

The variables can be set
by either typing them into
the fields, or selecting
them from the list and
clicking the Set button.

5. Click Okay to finish the
variable setup.
6. Choose Region or
Surface.
7. Click Create.

Page 263

ADVANCED USAGE
The resulting shock can be filtered by any of the threshold variables

1. Select the variable to filter by.
2. Set the Threshold filter to remove the portion of the shock
surface or region that is greater or less than the specified
threshold value.
3. Enter a threshold value
- or 3. Slide the slider to a new threshold value
4. The shock is usually defined in a very narrow band, so the
slider min/max values may need to be adjusted by either
entering new values in the min/max fields, or clicking on the
up/down buttons to change by an order of magnitude.

OTHER NOTES
See Other Notes in the Shock Surface/Region Create/Update section of the User Manual for options on how to prefilter flow field regions, and/or post-filter shock regions via a specified mach number. Also to apply the transient
correction term for moving shocks when using the shock Region method.
Shock Surface feature extraction does not work with multiple cases.

SEE ALSO
User Manual: Shock Surface/Region Create/Update

Page 264

Create Material Parts

INTRODUCTION
A Material Part can be created as either a domain or an interface.
A material Domain is a solid region (or regions) composed of one or more specified materials. Parts with 2D
elements yield 2D material elements, and parts with 3D elements yield 3D material elements.
A material Interface is a boundary region (or regions) between adjacent materials composed of at least two or more
specified materials. Parts with 2D elements yield 1D material elements, and parts with 3D elements yield 2D material
elements.
The Material Part feature can be used to isolate specified elemental regions of interest in data sets with material
fractions.

BASIC OPERATION
For Material Domain (for Smooth Method):
1. Click the Material Parts creation icon.

2. Select the parent model part(s).
3. Set Type to Domain.
4. Select 1 or more materials.
5. Click Create.

For Material Interface (for Smooth Method):
1. Click the Material Parts creation Icon.

2. Select the parent model part(s).
3. Set Type to Interface.
4. Select 2 or more materials.
5. Click Create.

Page 265

SEE ALSO
User Manual:
Material Parts Create/Update
In Section 11.1, EnSight Gold Casefile Format, see EnSight Gold Material Files Format

Page 266

Remove Failed Elements

INTRODUCTION
A variable can be used within EnSight as a means of removing elements that have “failed”. This failure is a ‘deep’
failure in that elements are not just visually removed on the client, but is also removed for all calculations on the
server. For example, the volume of a part calculated using the calculator will only include the non-failed elements. If
you only need to visually fail the elements consider Element Blanking.
The failure criteria can be something as simple as a variable with two states (one state to indicate the element is
failed, and the other state to indicate that the element is not failed), or it can be a variable (such as a Von Mises
stress/strain) threshold for which you specify limiting values and conditions for failure. The failure variable must be
a per-element variable. Also, this operation can only be performed on model parts. So if its effect is desired on
created parts, such as clip planes or isosurfaces, one should apply this operation to the model parent parts of the
desired created parts.

BASIC OPERATION
To use a per-element variable for removing failed elements:
1. Select the model part(s) to use.
2. Select Part Mode.
3. Click on the Failed elements button.
4. Select the per-element variable to
use for failure (in this example we use
Failure_Stress).
5. Set the desired condition(s) and
value(s) (in this case we fail if the
Failure_Stress is greater than 0.70)
6. Click Apply

Those elements which satisfy the
failure criteria will be removed from the
model.

Page 267

ADVANCED USAGE
EnSight’s User-defined reader API is capable of dealing with designated failure variables and the failure values and
conditions. Thus, a reader can be set up to use failure conditions that solvers provide and automatically apply the
failed element operations for you. An example of this is the LS-DYNA3D reader provided with EnSight.
Note the extra GUI option provided by this reader,
entitled: “Remove Failed Elements”.
By checking this option, a “Delete_Flag” variable is
created, and the failed element feature of EnSight will
be automatically on - with the conditions and values set
that will remove the failed elements that the solver
flagged as such. (Which for LS-DYNA3D is a value
equal to 0.0 in the Delete_Flag variable)

SEE ALSO
How-To Read User Defined
User Manual: Failed Elements

Page 268

Do Element Blanking

INTRODUCTION
EnSight allows you to pick elements in the model and make them disappear - “blank them out”. This may be desirable
if you want to peek inside of certain parts or remove portions of a part (without making the entire part invisible or
transparent). Element blanking is only visual removal on the client. For example the calculated volume does not
change if some elements are blanked. Element blanking is a temporary state that can easily be “cleared” - making
the elements visible again.

BASIC OPERATION
Using picking to do element blanking:
1. Set the pick action to “Pick element(s) to
blank”.
2. Select part(s) in the part list that you wish
to operate on.
3. Place the mouse pointer over the element
you wish to blank out and press the “p” key
to blank the element.
You will see the element under the mouse
disappear as you do the picking.
4. To cause the elements to reappear, click
the Element blanking/visibility icon and click
the clear button in the dialog which comes
up.

Note that blanking can be done directly using the
mouse if you change the mouse and keyboard
settings. For example, the preferences can be
set to blank using a middle mouse button click
on the part. Edit > Preferences > Mouse and
Keyboard.

Page 269

Also, the selection tool can be used to do element blanking on a larger scale:
1. Select the part(s) on which to do element
blanking.
2. Click on the Selection tool icon to turn on the
tool.
3. Position the tool as desired.
4. Click on the blanking icon.
5. Choose the criteria to use for blanking: inside
or outside (inside or outside the box) and top
or all (top is just the first visible layer, all is to
blank all elements in a direction perpendicular
to box.
6. Click on the element blanking eraser symbol
at the upper left of the tool.
To undo the blanking, click the Clear or Clear all
parts button.

Results in the following:

Note
The element IDs are used to tag visibility. These tags are preserved through timestep changes. If the elements
change IDs (perhaps changing connectivity) then EnSight will continue to use those same IDs which may result in
invisible elements at different locations.

SEE ALSO
How To Use Selection Tool
User Manual: Element Blanking

Page 270

Use Point Parts

INTRODUCTION
A point part is a part composed only of nodes. It can be read in as a model part or can be created through the use of
the Point Part feature. In order to create the part, a series of point locations must be defined. The point locations can
be read from an external file, or can be created by placing the cursor tool at desired locations and adding points. You
can later edit the locations of, or delete any of the points. When you select a parent part and click Create, a new part
with only nodes is created. This type of part can represent probes in the data, or lends itself well to meshing into a 2D
or 3D part. As the per-node variables of the model parts are mapped to the point part locations, it is also a great way
to write out nodal variable information (using File->Save->Geometric Entities) for further calculations. Note if a parent
part has per element variables then they must be moved to the nodes using the calculator functon ElemToNode.

BASIC OPERATION
2. Click the Point Part icon.

1. Select the parent part.

5. Click Create.
6. To create a mesh
from a point part,
click on the
Advanced button.

3. Make the cursor tool visible.
4. Move the cursor to the desired spot.
(Interactively or by using the Transformation Editor.)
and
Click the Add Point (at cursor) button.
(Repeat as many times as needed)
OR
4. Click the Load points from file... button.
(Which will bring up the file select dialog)
and select a file that contains the desired
points.
(See Section 11.17 Point Part File Format in the User Manual)

A simple sample of a Point Part file:
#Version 1.0
#EnSight Point Format
-.5, -.5, .5
-.5, .5, .6
.5, -.5, .7
.5, .5, .4
-1.5, -1.5, .5
1.5, 1.5, .3
2.25, 2.1, 1.5

SEE ALSO
User Manual: Point Parts Create/Update

Page 271

Page 272

Create and Manipulate Variables
Activate Variables

INTRODUCTION
When a results dataset is read into EnSight, associated variables are noted and listed in the Main Variables List.
However, a variable will remain deactivated (not loaded into memory) until some operation requires it or it is explicitly
activated (read into memory).
If an active variable is no longer required, you can deactivate it and free the associated memory.

BASIC OPERATION
Variable Activation
In most instances, variables are automatically activated as required. For example, if you create a contour using a
deactivated variable, EnSight will automatically activate the variable prior to creating the contour.
You can also activate variables explicitly using the Feature Detail Editor for Variables.
1. Open the Feature Detail Editor for Variables.

You can open this dialog in several ways. You can
do Edit > Variables editor... from the main menu
or
double click the Color/transparency icon in the Part
mode icons
or
single click the calculator feature icon

2. Select the variable(s) you wish to activate.
3. Click the Activate button.
OR
2. Click the Activate All button to
activate all variables in the list.

The (*) in the variable listing indicates
that the variable is currently loaded.

Page 273

Variable Deactivation
Variables are never deactivated automatically. To deactivate a variable:
1. Open the Feature Detail Editor for Variables.
You can open this dialog in several ways. You can
do Edit > Variables editor... from the main menu, or
double click the Color/transparency icon in the Part
mode icons, or after single clicking the Color/
transparency icon, you can double click on one of
the variables in the list of the Part color, lighting, &
transparency dialog.

2. Select the variable(s) you wish to deactivate.

3. Click the Deactivate button.
Note that variable deactivation can result in the modification or deletion of parts. If this is the case, you will be
asked to confirm the deactivation. A part could be modified if it used the deactivated variable for coloring. A part
could be deleted if it was based on the deactivated variable (such as a contour or an isosurface).

SEE ALSO
How To Edit Color Palettes, How To Create New Variables
User Manual: Variable Selection and Activation

Page 274

Create New Variables

INTRODUCTION
EnSight provides a powerful capability to derive new variables from existing variables and parts. For example, in a
fluids dynamics problem, if you have momentum, density, and stagnation energy you can calculate temperature,
Mach number, pressure, or velocity. In addition to the built-in functions, you can also compose your own functions
using the equation editor in conjunction with previously defined variables.
This article is divided into the following sections:
Introduction
Variable Creation
Examples of Expressions
Built-in Function Reference
Extended CFD Variables

BASIC OPERATION
Introduction
EnSight provides five distinct types of variables:
Constant

A constant variable is a single value. Constants do not vary across a part
although a constant can vary over time. Examples include Analysis_Time,
Temperature[123] (the value of temperature at node 123), Stress{3}[321]
(the value of stress at node 321 at time step 3), or the value of a function
that produces a constant (e.g. Area).

Scalar

A scalar variable is a set of values: one for each node or element of the
applicable part(s). Examples include Pressure, Velocity[Z] (the Z component
of velocity), Stress{3} (the value of stress at time step 3), or the value of a
function that produces a scalar (e.g. Flow)

Vector

A vector variable is a set of values: three (the X,Y,Z components) for each
node or element of the applicable part(s). Examples include Velocity,
Velocity{3} (the value of velocity at time step 3), Coordinates (a given
variable equal to the XYZ coordinate at a node), or the value of a function
that produces a vector (e.g. Vorticity).

Tensor

A tensor variable is a set of values: six (if symmetric) or nine (if asymmetric),
for each node or element of the applicable part(s). Tensor variables can be
represented by Tensor Glyphs directly, and within the variable calculator
eigenvalues, eigenvectors, determinant, VonMises or Tresca, etc. can be
computed.

Complex

A complex variable, which within Ensight can be either scalar or vector,
includes the real and imaginary portions of the values. The variable
calculator allows the user to compute things like modulus, argument,
transient response, etc.

Variables are either given (read from the dataset or automatically provided by EnSight) or computed (derived from
existing variables during an EnSight session). The variable type and whether it is given (shown as “Gvn”) or
computed (shown as “Cmp”) are shown in the Variables list in the Feature Detail Editor for Variables. If you have any
element-based variables in a model, the variable names in the Main Variables list will be preceded by “(E)” for
element-based or “(N)” for node-based.
Every non-constant variable (both given as well as computed) has an associated color palette that defines the
mapping from variable values to color. These palettes can be edited to change the mapping (see How To Edit Color
Maps for details). The value of a constant variable can be displayed as a text string in the Graphics Window (see
How To Create Text Annotation for details).
For time-dependent data, calculated variables will automatically recalculate when the current time step is changed.

Page 275

Variable Creation
Derived variables are easily created using the Feature Detail Editor Variable Calculator. To create new variables:
1. Double-click the Variable Calculator icon
in the Feature Icon bar to open the Feature
Detail Editor (Calculator).

3. Select the desired tab to either use
predefined functions or define your own
equation using math operators and
functions.
Prefedined functions Tab:
When you select a function, the Variable Name
field (at the top of the section) is loaded with the
name of the function. This will be the name of
the variable as seen in the Main Variables list.
You can change this name by entering a new
value (and pressing return).
A description of the function parameters appears
directly below the tab.
Dynamic Instructions for properly composing the
required parameters will appear to the right of
the list.
The expression is built in the Working
Expression section. As you insert parameters,
they are automatically added to the expression
and the instructions for the next parameter will
appear. Parameters can be inserted as follows:
Parts: by selecting the desired part(s) in the
Main Parts list (and clicking Next) or by entering
the part number in the field provided and
selecting Next. Note that the place holder “plist”
appears in the expression denoting the list of
currently selected parts.
Variables: by clicking on the desired variable in
the Which Variable list.
Constants/other: by typing the desired constant
or other text directly into the field provided or by
clicking the desired item in the Calculator
keypad (which is accessed via the “#” button).
4. Follow the instructions to build the desired
expression and then click Evaluate.

Page 276

Define equation Tab:
Alternatively, you can build your own equation
by selecting variables, math functions,
operators, and numbers as desired.
Once you have the desired equation in the
Working Expression field, and a name in the
Variable name field - click Evaluate.

Examples of Expressions
The following examples demonstrate usage of the variable calculator. In each case, first enter a name in the Variable
Name field and click in the Working Expression area to activate it. The examples assume that Analysis_Time (a given
constant variable if the dataset is transient), pressure, density, and velocity are all given variables.
Expression
-13.5/3.5

Description and How to Build
A simple constant.
To build, either type the text on the keyboard or click in the Calculator keypad.

Analysis_Time/60.0

A constant variable. Assuming the solution time was given in seconds, this expression will
provide a variable giving the time in minutes.
To build, select Analysis_Time from the Active Variable list and either type or click /60.0

velocity*density

Momemtum – a vector variable.
To build, select velocity from the Active Variable list, click or type *, and select density
from the Active Variable list.

SQRT(pressure[73]*2.5)
+ velocity[X][73]

Square root of (pressure at node 73 * 2.5 + the X component of velocity at node 73)
To build, select SQRT from the Math function list, select pressure from the Active Variable
list, click or type [73]*2.5)+, select velocity from the Active Variable list, and click or
type [X][73].

Page 277

Expression

Description and How to Build

velocity^2

You have to be careful here. velocity^2 is NOT equal to DOT(velocity,velocity). A vector *
vector in EnSight is performed component-wise (x-component * x-component, ycomponent*y-component, and z-component*z-component). The magnitude of this
expression is SQRT(x-component^4 + y-component^4 + z-component^4) which is NOT the
square of the magnitudes. If you are looking for a scalar result for the square of the velocity,
use DOT(velocity,velocity), or, for velocity magnitude, use RMS(velocity) or
SQRT(DOT(velocity,velocity)), or SQRT(velocity[x]*velocity[x] +
velocity[y]*velocity[y]+velocity[z]*velocity[z]).

pressure{19}

Scalar variable equal to pressure at time 19. This variable will not change if the current
time step is changed.
To build, select pressure from the Active Variable list and click or type {19}.

MAX(plist, pressure)

Constant variable equal to the maximum value for pressure over all nodes of all parts in
plist.
To build, select MAX from the General function list and follow the instructions in the Feedback
area.

(pressure/max_pres)^2

Scalar variable equal to squared normalized pressure.
To build, first calculate the MAX constant variable as described in the preceding example
(here named max_pres). Click or type (, select pressure from the Active Variable list, click
or type /, select max_pres from the Active Variable list, and click or type)^2.

Since EnSight can compute only one variable at a time, one must break down involved equations into multiple
smaller ones, using temporary or intermediate variables.
Calculator limitations include the following:
1. The variable name cannot be used in the expression. The following is invalid:
temperature = temperature + 100

Instead use:
temperature2 = temperature + 100

2. The result of a function cannot be used in an expression.
(pressure / MAX(plist,pressure) )^2

Instead use two steps. Define p_max as:
MAX(plist,pressure)

then define norm_press_sqr as:
(pressure / p_max)^2

3. Created parts (or changing geometry model parts) cannot be used with a time calculation (using { }).
4. Calculations occur only on server-based parts. Client-based parts are ignored, and variable values may be
undefined.

Page 278

Built-in Function Reference
Although all built-in functions are listed here, consult the User Manual for the complete definition of a function.
EnSight provides the following built-in general variable calculation functions:
Function
Area
Boundary Layer Cf at Wall
Displacement
Thickness
Distance to
Value from Wall
Momentum
Thickness
Thickness
Y1 off Wall
Case Map
Coefficient
Complex
Argument
Conjugate
Imaginary
Modulus
Real
Transient
Response
Curl
Density
Distance Between 2 Nodes
Divergence
Dynamic Pressure
Element to Node
Energy, Total
Enthalpy
Entropy
Flow
Rate
Fluid Shear
Stress
Max
Force
on 1D part
Gradient
Approximation
Tensor
Tensor
Approximation
Helicity
Density
Relative
Relative Filtered
Iblanking Values
Kinetic Energy
Length
Line Integral
Log of
Density
Normalized
Pressure
Temperature
Mach Number
Make Scalar at Elements

Abbreviation (if
any)

Description

BL_CfWall
BL_DispThick

Surface area
Boundary Layer Cf at the wall
Boundary Layer displacement thickness

BL_DistToValue

Boundary Layer distance to value from the wall

BL_MomeThick

Boundary Layer momentum thickness

BL_Thick
BL_Y1Plus
CaseMap
Coeff
Cmplx

Boundary Layer thickness
Boundary Layer Y1 off wall
Map values of a variable from one case onto the nodes of another case.
Coefficient
Create complex variable from variables representing the real and
imaginary portions.
Argument of complex variable
Conjugate of complex variable
Imaginary portion of complex variable
Modulus of complex variable
Real portion of complex variable
Complex transient response

CmplxArg
CmplxConj
CmplxImag
CmplxModu
CmplxReal
CmplxTransResp

Dist2Nodes
Div
PresDynam
ElemToNode
EnergyT

Curl of a vector
Density
Distance between two nodes
Divergence
Make node-based variable from element-based variable (via average)
Total Energy

Integrated flow through 1D/2D part
FlowRate
FluidShear
FluidShearMax

Fluid shear stress
Max of fluid shear stress
Force Vector
Force1D
Force Vector on 1D part
Grad
3D gradient of a variable
GradApprox
Linear, closed-form gradient approximation
GradTensor
3D tensor gradient
GradTensorApprox Linear, closed-form tensor gradient approximation
HelicityDensity
HelicityRelative
HelicityRelFilter
IblankingValues
KinEn
IntegralLine
DensityLogNorm
PresLogNorm
TemperLogNorm
MakeScalElem

Scalar that is the iblanking flag per node
Kinetic energy
Summed length of all 1D elements
Integral over 1D elements

Mach number
Scalar created, by placing a constant value at each element

Page 279

Function
Make Scalar at Nodes
Make Vector
Massed Particle Scalar
Mass Flux Average
Maximum
Minimum
Moment

Abbreviation (if
any)
MakeScalNode
MakeVect
MassedParticle
MassFluxAvg
Max
Min

Moment Vector

MomentVector

Momentum
Node To Element
Normal
Normal Constraints
Normalized
Density
Enthalpy
Pressure
Stagnation
Density
Stagnation
Enthalpy
Stagnation
Pressure
Stagnation
Temperature
Temperature
Vector
Offset
Field
Variable

Momentum
NodeToElem

Pitot

NormC
DensityNorm
EnthalpyNorm
PresNorm
DensityNormStag

Stream Function
Surface Integral
Swirl
Temperature
Temporal Mean

Scalar created, by placing a constant value at each node
Build a vector variable from scalars
Massed particle scalar
Find spatial max of variable over part(s) at current time
Find spatial min of variable over part(s) at current time
Moment component of a force component based on the current position
of the Cursor Tool. This is a constant.
Moment component of a force component at each node of selected
parts. This is a field of vectors.
Make an element-based variable from node-based (via average)
Surface normal vector
NC

EnthalpyNormStag
PresNormStag
TemperNormStag
TemperNorm
NormalizeVector
OffsetField
OffsetVar

PresPito
PresPitoRatio
Pressure
Pres
Coefficient
PresCoef
Rectangular To Cylindrical Vector RectToCyl
Server Number
ServerNumber
Shock Plot3d
Sonic Speed
Spatial Mean
Speed
Stagnation

Description

Vector field expressed as unit vectors.
Offset distance field (from boundary)
Variable Value offset from boundary of part into the field (placed on
boundary)

Pressure
Pressure Ratio

ShockPlot3d
SonicSpeed
SpaMean
Density
Enthalpy
Pressure
Pressure
Coefficient
Temperature

Pressure
Calculate vector in cylindrical coordinates
Per Element variable created that is the server number containing the
element

Mean of a variable over a part
Magnitude of velocity

DensityStag
EnthalpyStag
PresStag
PresStagCoef
TemperStag
Stream
IntegralSurface
Swirl
TempMean

Stream
Integral over 2D elements
Temperature
Mean of a variable over time

Page 280

Function

Abbreviation (if
any)
TensorComponent
TensorDeterminant
TensorEigenvalue
TensorEigenvector
TensorMake
TensorMakeAsym

Component of a tensor variable
Determinant of a tensor variable
Eigenvalue of a tensor
Eigenvector of a tensor
Make symmetric tensor from variables representing components
Make asymmetric tensor from variables representing components

Total Pressure
Velocity
Volume

TensorTresca
TensorVonMises
PressT
Velo
Vol

Tresca failure theory of a tensor
Von Mises failure theory of a tensor
Total pressure
Momentum/density
Volume of 3D elements

Volume Integral
Vorticity

IntegralVolume
Vort

Integral over 3D elements
Vorticity

Tensor

Component
Determinant
Eigenvalue
Eigenvector
Make
Make
Asymmetric
Tresca
Von Mises

Description

The following standard math functions are also available:
Function

Abbreviation

Function

Abbreviation

Absolute Value

ABS

Root Mean Squared

RMS

Arccosine

ACOS

Round

RND

Arcsine

ASIN

Sine

SIN

Arctangent

ATAN

Square Root

SQRT

Arctangent (y / x)

ATAN2

Tangent

TAN

Cosine

COS

Cum Normal Distribution

CDF_NORM

Cross Product

CROSS

Normal Prob Density

PDF_NORM

Dot Product

DOT

Student T Cum Distrib

CDF_T

Exponent

EXP

Student T Prob Density

PDF_T

Greater Than

GT

F Cumulative Distribution

CDF_F

Less Than

LT

F Probability Density

PDF_F

Log Natural

LOG

Cum Chi Square Distrib

CDF_CHISQU

Log Base 10

LOG10

Chi Square Prob Density

PDF_CHISQU

For information on the arguments (and equations), see General Functions or Math Functions in the User Manual.

Page 281

Extended CFD Variables
Rather than having to individually create the various common CFD variables, EnSight can automatically make them
available for use if the appropriate basis variables and constants have been provided. This can be accomplished
after loading the model with the Extended CFD Variable Settings Dialog:
1. From either the Variable or the Calculator
Feature Detail Editor, click the Extended
CFD Variables... button.

2. Select the variable name in the list and then
click the appropriate SET button.
For example, select Density in the list and then
click the SET button to right of the Density field.
3. After all variables and constants have been
specified, click Show Extended CFD
Variables.
4. Click Okay.
The common CFD variables will now be listed in
the main variables list. Note that they will NOT
actually be computed until activated.

If you have a “standard” PLOT3D Q file, the above
process can be accomplished automatically by
starting EnSight with the “-cfd” option on the
command line.

SEE ALSO
How to Edit Color Maps
User Manual: Variable Creation

Page 282

Extract Boundary Layer Variables

INTRODUCTION
EnSight can compute the following boundary layer parameters:
boundary layer thickness
displacement thickness
momentum thickness
shape parameter
skin friction coefficient

named:

(bl_thickness)
(bl_displ_thickness)
(bl_momen_thickness)
(bl_shape_parameter)
(bl_skin_friction)

You must have a 2D surface in a 3D field and specify the 2D surface as the parent part(s).
For a complete description of these variables, refer to the User Manual section below.

BASIC OPERATION
1. Select the 2D parent part(s).
2. Click the Boundary Layer variable icon.

3. Bring up the dialog
defining the necessary
variables by clicking here.

4. Define either (Density
and Momentum) or
velocity.
The variables can be
set by either typing
them into the fields, or
selecting them from the
list and clicking on the
Set button.

6. Choose the method that
will be used to determine
the velocity outside the
boundary layer.

5. Click Okay to finish
the variable setup.

7. Click Create/Update.
This will create the five new
variables, which can be used for
further operations - such as part
coloring.

Page 283

OTHER NOTES
These variables and more are also individually available in the Variable calculator. See the Boundary Layer
Variables section of Chapter 4 in the User Manual
Note that the Freestream Density, and Freestream Velocity fields are for constant ‘upstream’ density and velocity
magnitude values (near flow inlet). They are only used for skin-friction coefficient, Cf.
Boundary Layer variables do not work with multiple cases.

SEE ALSO
How To Create New Variables
User Manual: Boundary Layer Variables Create/Update

Page 284

Edit Color Palettes

INTRODUCTION
All scalar and vector variables have an associated color palette that defines the mapping from variable values to
colors. These palettes can be easily edited to customize the mapping. Color palettes can also be saved to disk and
restored during a subsequent session.

BASIC OPERATION
The default color palette created for each variable has five Levels (with the minimum and maximum set to the range
of the variable at the time step selected when the variable was activated). The color ramp is a standard spectrum with
the five Levels set to (from min to max) blue, cyan, green, yellow, and red.
EnSight can display multiple color legends in the Graphics Window:

1. Click the Legend... button on the desktop.
2. Select the desired variable(s) in the list.
For vector variables, you can select magnitude (or click Show
Components to be able to select the components as well).

To remove a legend:
Repeat 1. and 2. above
or
You can remove all legends by clicking the All Off
button.
Color legends have a number of display attributes including size, position, and how/where the variable labels are
formatted. See How To Create Color Legends for details.

Page 285

The Palette Editor provides access to all aspects of variables including min/max information, histogram distribution,
and variable value mapping to color and transparency. :
1. Click the Color icon in the Part Mode bar to open
the Color Editor.
2. Click the Palette... button to bring up the Palette
Editor

3. Select the palette to be
edited from the pulldown

Grab the Minimum Palette
Value Slider
Type in a Minium Palette Value

Opens by default in Simple Tab

Palette Levels (and variable
values). Enter a new value if
desired. Click on Color to
change.

To change the colors associated with the
levels

Grab the Maximum Palette
Value Slider
Enter a Maximum Palette
Value
Update variable range using
a) extrema, b) selected
part(s) (note element
representation of part(s)
matters), c) currently visible
part(s) in selected viewport.
Enter desired number of
Levels in the palette (2 to 21)
Reverse colors/levels
Interpolate between two
levels. Enter the upper and
lower levels and click
interpolate to create the
intermediate levels.

4. Click on the color for the level you
wish to modify and select a new color
in the pop up dialog.
OR
5. Click the Invert colors button to invert the
color order
OR
6. Click on the File Tab and choose a new
palette and click Restore to load a new palette.

Page 286

ADVANCED USAGE
1. Double-click the Color icon in the Part mode bar to open the Color Editor, then click on the
Palettes... button.
2. Select Advanced Tab
A color palette is composed of color and opacity information at a set number of control points. By default,
EnSight creates the control points to be uniformly spaced and to have the same number as the number
of levels in the palette. You can decouple the control points from the levels by changing the Node Locking
option at the bottom of the dialog.
The background of the control point graphic contains a histogram distribution for the variable tied to the
palette. The small horizontal handle at the left of the image will scale the histogram information.
Now manipulate the Control Points
3. Select which component (Red, Green, Blue,
or Alpha) to manipulate.
Change the value of the Control Points
4. Click on a Control Point and type in a value in
the Value: field,
4. OR Click on the Control Point and drag it to a
new value. By default the movement of the
control point is limited such that only the
value can be changed. If you wish to move
the control points location you must unlock it
by untoggling the Node Locking option in the
Options tab
Add or Delete a Control Point
5. Right click on a control point to choose to
add or delete a control point. If adding a
control point, it will be added to the right of
the selected point.

7. Click on the Options Tab
8. The default is Type of
Continuous to interpolate
and smooth the color.

9. To create a color band for
each color in the texture,
change Type to Banded.
Reduce the number of
Colors per level to
coarsen the bands

6. For a large dataset, change ‘Update:’ to
Delayed. An Apply button will appear.
Changes will take effect when you click it.
10. You can specify how to handle
Undefined variable values. The default is
to display the Undefined value as the
color for 0. You can change this such
that Undefined values will be invisible.
11. Limit fringes: The default behavior is
for variable values outside the min/max
range to be mapped to the color/opacity
defined at the bottom and top of the
palette. You change this behavior such
that out of bound values are colored by
the part color or are set to invisible.
12. Change the alpha volume scale to affect
volume rendering
13. For transient data, toggle on and fill in
time range to use to rescale variable
extrema and recreate histogram over
time.

Page 287

Markers are single-colored level(s) overlaid on top of the
color palette designed to emphasize the distinction
between levels.
14. Click on the Markers Tab. Markers are divider
bands drawn in the color specified at the specified
variable value. They serve to divide your coloration
similar to isocontours.
15. Choose the color, the width and the maximum
number of markers
16. At the Add: pulldown, choose one of the
following to add markers at At levels (adds a marker
at each level value), At value (adds a single marker
at the value indicated), or Uniformly (adds marker
uniformly if you enter a value into the How Many
field that appears.
17. Markers remain until cleared.

EnSight includes a number of predefined palettes
available for loading.
18. Choose a palette.
19. Click restore to load it.
If the new number of levels do not match the current
number of levels a dialog will pop up to ask whether you
want the new number of levels or the current.

OTHER NOTES
SEE ALSO
How To Create Color Legends, How To Create New Variables, How To Create Contours
User Manual: Variable Summary & Palette and Palette File Formats

Page 288

Use Volume Rendering

INTRODUCTION
Most of the visualization techniques in EnSight use points, lines, and surfaces to represent data, requiring volumetric
data to be subsampled in some way. Volume rendering is a visualization technique that allows the user to view an
entire volume of data at once, without having to slice the data in any way. The process involves finding all cells that
overlap each pixel and accumulating a color for that pixel from the color and transparency of each cell. Volumes can
be constant colored, but more often you will color the volume using a palette corresponding to a variable or a variable
component. Color palettes include transparency ("alpha") values, allowing control of transparency based on variable
value.

BASIC OPERATION
1. Select the parent part.

5. Choose Volume Rendering.

2. Open the color dialog.
3. Color the part by a variable

4. Select the
element settings.

Volume rendering is one of several "element representations" for a part. Results are generally loaded into EnSight by
default in Border, Feature Angle, or Full representation. These representations include only point, line, or surface
data. The "volume" element representation will activate volume rendering for a part. Just as for surfaces, the part
color dialog can be used to control the color and opacity of the volume. You can color the volume by a scalar, vector,
or vector component, and the colors will be assigned based on the palette.

Page 289

ADVANCED USAGE
EnSight provides advanced control of volume rendering. You can control the volume rendering magnitude of each
level of the variable palette by adusting the alpha value (shown as an A in the Palette Editor). The alpha value is the
opacity/intensity of the particular level when volume rendered. This means that you can emphasize select variable
levels in your volume rendering coloration by specifically increasing the alpha magnitude of these select levels. You
can also scale up the entire alpha by adjusting a multiplier value.

6. Click on the Palette button.

9. If the volume looks nearly
invisible then increase the
alpha scale uniformly raise
the opacity level.

7. Click on the control points
with the left mouse button
and drag them upward.
8. Notice the opacity of the
variable values at these levels
is scaled upward creating
emphasis in
the graphics
screen and in
the legend

OTHER NOTES
Volume rendereing requires a DirectX 10 capable graphics card. Newer cards with more memory and up-to-date
software drivers will perform best. Volume rendering will use roughly 1GB of graphics memory per 10M tetrahedra.
Other cells will be decomposed into multiple tetrahedra. EnSight will disable volume rendering when it encounters
archaic graphics card hardware. Because volume rendering exercises a large amount of the OpenGL functionality
remote rendering problems are very likely, therefore this remote rendering is not supported.

SEE ALSO
See How to Change Visual Representation, How To Edit Color Maps for more information.

Page 290

Query, Probe, Plot
Get Point, Node, Element, and Part Information

INTRODUCTION
EnSight provides many methods for extracting exact quantitative data from your results. Specific information about
nodes, elements, parts, IJK locations, or arbitrary points can be displayed.

BASIC OPERATION
Show Point Information
To show information about an arbitrary point:
1. If your data is transient, set the desired time using the Solution Time Quick Interaction area (Edit >
Solution Time Editor...).
2. If you have multiple Cases, select the desired case using Case > casename.
3. Position the Cursor Tool to the desired location.
4. Select the desired part(s) in the Main Parts List. The query will only be successful if the Cursor Tool
is found within an element of a selected part.
5. Select Query > Show Information > Cursor.
The query results will be printed to the EnSight message window, which will pop up.
It can also be accessed from the Info icon.
The following shows sample output from a point query:
Point (6.19810e-01,2.77589e-01,2.41451e-01)(In Frame 0) Query Information.
Found in structured part # 2.
Found in element # 168379.
Closest node # 1782 (within the element)
Value for Variable density is 9.96230e-01.
Values for Variable momentum are:
x=3.03989e-01,y=-1.42727e-02,z=8.51241e-02,mag=3.16005e-01.

Show Node Information
To show information about a specific node, you must have either given or automatically assigned node labels for your
data. You must also know the number of the node of interest. If you do not know the number, you can display node
labels for the part or, if you know an element that contains the node, you can display element information for the
element (as described in the next section). To show node information:
1. If your data is transient, set the desired time using the Solution Time Quick Interaction area (Edit >
Solution Time Editor...).
2. If you have multiple Cases, select the desired case using Case > casename.
3. Select the desired part(s) in the Main Parts List. The query will only be successful if the specified
node is found in a selected part.
4. Select the variable(s) you wish to query in the Main Variables List (only node-based variables will be
queried).
5. Select Query > Show Information > Node. The Query Prompt dialog opens. Enter the ID number of
the desired node in the text field and click Okay.
The query results will be printed to the EnSight message window, which will pop up.
It can also be accessed from the Info icon.
The following shows sample output from a node query:
Node 123 Query Information.
Coordinates (In Frame 0) are: (-2.00000e+00,0.00000e+00,1.19320e+00)
Found in unstructured part # 1.
Values for Variable velocity are:
x=5.82290e-01,y=3.70160e-02,z=-1.82780e-03,mag=5.83468e-01.

Page 291

Show IJK Information
To show information about a specific IJK location for structured models:
1. If your data is transient, set the desired time using the Solution Time Quick Interaction area (Edit >
Solution Time Editor...).
2. If you have multiple Cases, select the desired case using Case > casename.
3. Select the desired part (one only) in the Main Parts List. The query will only be successful if the
specified IJK is found in the selected part.
4. Select the variable(s) you wish to query in the Main Variables List (only node-based variables will be
queried).
5. Select Query > Show Information > IJK. The Query Prompt dialog opens. Enter the values for the
desired IJK location in the text fields and click Okay.
The query results will be printed to the EnSight message window, which will pop up.
It can also be accessed from the Info icon.
The following shows sample output from an IJK query:
IJK 2 5 10 Query Information.
Node Id is: 26146
Found in iblanked structured part # 1.
Coordinates (In Frame 0) are: (4.72982e-01,1.64710e-01,6.50679e-02)
No variables active to show values at the IJK location.

Show Element Information
To show information about a specific element, you must have either given or automatically assigned element labels
for your data. You must also know the number of the element of interest. If you do not know the number, you can
display element labels for the part. To show element information:
1. If your data is transient, set the desired time using the Solution Time Quick Interaction area (Edit >
Solution Time Editor...).
2. If you have multiple Cases, select the desired case using Case > casename.
3. Select the desired part(s) in the Main Parts List. The query will only be successful if the specified
element is found in a selected part.
4. Select the variable(s) you wish to query in the Main Variables List (only element-based variables will
be queried).
5. Select Query > Show Information > Element. The Query Prompt dialog opens. Enter the ID number
of the desired element in the text field and click Okay.
The query results will be printed to the EnSight message window, which will pop up.
It can also be accessed from the Info icon.
The following shows sample output from an element query:
Element 321 Query Information.
Found in unstructured part # 2.
Type of element is 6 Noded triangle
Number of nodes is 6
Node IDs are: 1050 910 1054 1052 1053 1055
Neighboring Element Information is:
Element neighbor 318 is of type 6 Noded triangle
Element neighbor 322 is of type 6 Noded triangle

Page 292

Show Part Information
To show information about a part:
1. If your data is transient, set the desired time using the Solution Time Quick Interaction area (Edit >
Solution Time Editor...).
2. Select the desired part in the Main Parts List.
3. Select Query > Show Information > Part.
The query results will be printed to the EnSight message window, which will pop up.
It can also be accessed from the Info icon.
The following shows sample output from a part query:
Part 2 Query Information.
Unstructured part.
Number of nodes 2380
Minimum coordinate(In Frame 0) is (0.00000e+00,0.00000e+00,0.00000e+00)
Maximum coordinate(In Frame 0) is (3.80000e+01,1.20000e+01,0.00000e+00)
Min node label in part is (1)
Max node label in part is (2380)
Element Information is:
Element type: 6 Noded triangle, count = 1128.
Min element label in part is (1)
Max element label in part is (1128)

Note: In general client side parts (particle traces, profiles, vector arrows, contours) can’t be queried in this manner.
You will receive and error message like the following:
ERROR: The query of the part specified could not be completed.

Particle trace parts will give one bit of information - namely how many traces there are in the part. And a note will be
given informing you how to get a “dump” of the trace into the message window. Something like:
Part 2 Query Information
This part is a particle trace part
Part has 10 traces
Note:
For full trace dump into this window,
issue the following command in the command dialog:
test: full trace query ON
Then repeat this query.

SEE ALSO
How To Query/Plot, How To Probe Interactively.
User Manual: Show Information

Page 293

Probe Interactively

INTRODUCTION
EnSight provides an interactive query capability that displays variable data in the Graphics Window as you move the
mouse pointer over geometry, as you move the cursor tool within the model, or at specified node, element, ijk or xyz
locations. The probe can display the value directly under the mouse pointer (by interpolating the nodal values of the
applicable element) or search for and display the value at the node closest to the mouse pointer.

BASIC OPERATION
To probe interactively:
1. Click the Probe Icon (or select
Query > Interactive Probe...).
2. Set the Query pulldown to
desired operation.
3. Select the desired variable to
display.
Surface Pick: Interpolate to any picked
position on the surface of the model.
Cursor: Interpolate to location of cursor
tool within the model.
Node: At a specific node number.
IJK: At a specific IJK location.
Element: At a specific element number.
XYZ: At a specific XYZ location.

5. Enter a value controlling the number of
simultaneous probe markers displayed. Once
this number has been reached, the oldest
marker is replaced by each new marker.
6. If the selected variable is a vector variable,
you can specify which component (or the
magnitude) of the variable is displayed.
7. In addition to having the results displayed on
the model in the graphics window, you can
open a table that displays the results

4. If Query is set to Surface Pick,
you can select:
a) whether the probe will snap
to closest node or
b) use exact location.

8. When done, change the Query to None to
disable interactive probing.

And whether the information will
be sampled:
c) when you click the “p”
keyboard key or
d) continuously as you move
the mouse.
If Query is set to Node, Element,
IJK, or XYZ, enter ID or values
needed followed by Enter.
If Query is set to Cursor, move
the cursor tool to desired
location and press the “p”
keyboard key (while the mouse
is in the graphics window).

Page 294

Probe Display Attributes
Probes are displayed as a marker (sphere) and the query text label. The appearance of the marker and label can be
changed:
1. Click the Display
Attributes... button in the
Probe Quick Interaction
area.

Toggle visibility for the id label.
(Node id, element id, etc.)

Toggle visibility for the query
text label.

Toggle whether query text
labels are “always on top”
(never hidden by geometry) or
occluded by geometry that is
closer.

Set the color of the label.

Toggle visibility for the probe
marker.

Set the radius of all probe
markers.

Set the color of the marker.

See the Elements surrounding the query
It is possible to extract the elements that contain the query
locations, if element ids exist:
1. Click the Display Attributes... button in the Probe
Quick Interaction area.
2. Click the up arrow.
An expansion factor of 1 indicates that the elements that
contains the query will be extracted and shown.
3. Click the up arrow again.
An expansion factor of 2 indicates that the elements
from the step 2 will be shown along with the elements
that neighbor these elements.
Since the expansion factor feature uses a subset part, if
you wish to display the subset part differently (such as
turn on node labels) this can easily be done through the
subset part attribute editing. The name of the subset
part in the part list will be "Query show expand".

4. If you wish to keep the subset part that was the
result of the display expansion factor setting you
may do so when you turn off the interactive query.
A pop-up dialog will ask you if you wish to keep or
delete the expansion factor subset part.

Page 295

OTHER NOTES
Note that interactive query actions do not generate corresponding command language!
When in query mode and using the ‘p’ key to pick a query location, other picking options that use the ‘p’ key are
disabled (such as the picks in Part Mode: Part, Cursor, Line, Plane, and LookAt Point).
The Quick Interaction area contains all the attributes that can be set for Probe Interactively. There is no Probe
Feature Detail Editor.
Even though it is not shown in the dialogs above, the “Time” variable is also available. This time variable is the
integration time for particle traces. Thus, it is only defined and useful when probing particle traces. For other part
types it will be undefined.

SEE ALSO
How To Query/Plot
User Manual: Interactive Probe Query

Page 296

Query/Plot

INTRODUCTION
EnSight can perform a number of different kinds of queries over time or space. The result is a Query Entity that can
be plotted using EnSight’s built-in Plotting facility or that can be printed as a table or written to a disk file.

BASIC OPERATION
One first must create query items, which can be any of the following types:
At Line Tool Over Distance.
At 1D Part Over Distance.
On a Spline Over Distance

At Node Over Time
At Element Over Time
At IJK Over Time
At XYZ Over Time
At Minimum Over Time
At Maximum Over Time
By Scalar Value

By Operating on Existing Queries
Read From An External File
Read from server file

As one of these is selected, the Quick Interaction Area changes to reflect the information needed (such as variable to
use) for the selected type. One can control whether the query entity will be a curve or a scatter plot by the choice for
Variable 1 and 2.
Query entities can be printed to the Status History Area, saved to a file, deleted, or plotted.

Sample Query Creation and Plot (At Maximum Over time)
2. Click the Query/Plot icon (or select
Query > Over Time/Distance...).

1. Select the part to query.
3. Select the Sample type for the
query.
4. Select the variable(s) for
Variable: 1.
Note: for max or min over time
you can select multiple variables
to query simultaneously over time
for efficiency.
Leave Variable: 2 as None and it
will default to Time, because of sample type.
5. Click Create

Page 297

6. Click Plot
7. Select the Query Item to
plot.
8. Click New Plotter.
Note: If any previous plotter has
the correct type, it will show up
in the list and can be selected
instead of creating a new one, if desired.
The plot will be displayed in the graphics window and will be listed in the Plotters Of Query’s Type list.
For more information on plotting, see the Plotting section towards the end of this How To.

Managing Query Entities
The Quick Interaction area provides various controls for managing existing Query Entities:
List of current Query
Entities. Selected items are
operated on by the following
actions.
Plot the selected Query
Entity as described above.
Append the text of the selected Query Entity to the
Status History window.

Save the selected Query Entity to a disk file, either as
xy data or in a formatted report-like manner.

Note that previously created and saved query entities are
restored through the use of the Read From An External
File query Sample option.

Update the selected query when any of
its attributes or have been modified.

Delete the selected Query Entity.
For various queries, marker visibility, as
well as size and color can be controlled
here as well.

Page 298

Over Distance Queries
EnSight can perform queries at uniform points along the line tool, at nodes along a 1D part, or at uniform points along
a spline. One-dimensional parts include model parts consisting of bar elements, 1D (Line) Clips, and particle traces.

At Line Tool Over Distance.
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “At Line Tool
Over Distance”
2. Select the variable to query over
the distance in “Variable: 1”.
Leave “Variable: 2” as None unless you want a scatter
query of two different variables along the line tool.
3. Optionally, select the Distance option desired,
number of points along the line, and modify the tool
location if needed.
4. Click Create

At 1D Part Over Distance.

1. Select the part containing only 1D elements.
2. Select Sample as “At 1D Part Over Distance”
3. Select one variable to query in “Variable: 1”.
4. Optionally modify Distance, origin and multiple segment attributes.
5. Click Create.
For the two over distance query types, the variable is plotted against the selected “Distance” metric. The node with
the lowest node ID number is queried first. Since the nodes for 1D part over distance are not necessarily evenly
spaced, the reported distance is one of the following:
Distance In Setting
Arc Length
X Arc Length
Y Arc Length
Z Arc Length
From Origin
X From Origin
Y From Origin
Z From Origin

Reported Distance
The distance along the part from the first node to each subsequent node (i.e. the
sum of the 1D element lengths)
The X coordinate value of each node accumulated from the start
The Y coordinate value of each node accumulated from the start
The Z coordinate value of each node accumulated from the start
The distance from the origin
The X distance from the origin
The Y distance from the origin
The Z distance from the origin

If the 1D part contains more than one set of contiguous 1D elements (such as a particle trace from a Line emitter), the
resulting query will contain one plot entity for each set.

Page 299

On a Spline Over Distance

After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as "At spline over
distance"
2. Select the variable to query along
the spline
3. Select the spline to query
4. Optionally, select the Distance option desired and the number of
points along the spline.
5. Click Create

Over Time Queries
For transient dataset, EnSight can query the variable values over a range of time at a particular node, element (or
specific IJK coordinate for structured data) or an arbitrary point. You can also search the minimum or maximum of a
variable over all nodes over a time range.

At Node Over Time
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “At Node
Over Time”
2. Select one variable to query
over time in “Variable: 1”.
Leave “Variable: 2” as None unless you want a scatter query of two different
variables over time.
3. Enter the Node ID.
4. Optionally, change the number of Samples (defaults to number of time
steps), and whether to sample by Value of FFT.
5. Click Create

Page 300

At Element Over Time
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “At Element
Over Time”
2. Select one variable to query
over time in “Variable: 1”.
Leave “Variable: 2” as None unless you want a scatter query of two different
variables over time.
3. Enter the Element ID.
4. Optionally, change the number of Samples (defaults to number of time
steps), and whether to sample by Value of FFT.
5. Click Create

At IJK Over Time
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “At IJK Over
Time”
2. Select one variable to query in
“Variable: 1”.
Leave “Variable: 2” as None unless you
want a scatter query of two different variables over time.
3. Enter IJK for the point.
4. Optionally, change the number of Samples (defaults to number of time
steps), and whether to sample by Value of FFT.
5. Click Create

At XYZ Over Time
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “At XYZ Over
Time”
2. Select one variable to query over
time in “Variable: 1”.
Leave “Variable: 2” as None unless you want a scatter query of two
different variables over time.
3. Either type in the desired xyz location or place the cursor where
desired in the model, either through picking, or other transformation
methods and click the cursor Get button.
4. Optionally, change the number of Samples (defaults to number of
time steps), and whether to sample by Value of FFT.
5. Click Create

Page 301

At Minimum Over Time
After selecting the part to query
and clicking the Query/Plot icon
1. Select Sample as “At
Minimum Over Time”
2. Select variable(s) to query
over time in “Variable: 1”.
Note: for max or min over time you can select multiple variables to query
simultaneously over time for efficiency.
Leave “Variable: 2” as None unless you want a scatter query of two different
variables over time.
3. Optionally, change the number of Samples (defaults to number of
time steps), and whether to sample by Value of FFT.
4. Click Create

At Maximum Over Time
After selecting the part to query
and clicking the Query/Plot icon
1. Select Sample as “At
Maximum Over Time”
2. Select variable(s) to query
over time in “Variable: 1”.
Note: for max or min over time you can select multiple variables to query
simultaneously over time for efficiency.
Leave “Variable: 2” as None unless you want a scatter query of two different
variables over time.
3. Optionally, change the number of Samples (defaults to number of
time steps), and whether to sample by Value of FFT.
4. Click Create

By Scalar Value
After selecting the part to query and
clicking the Query/Plot icon
1. Select Sample as “By Scalar Value”
2. Select the two variables you wish to
form the query from.
3. Select the desired scalar variable
and value
4. Click Create

Page 302

Scatter Query Example
A scatter query is a query of
one variable against another.

Everything is done like a
regular query except you
select another variable in the
Variable: 2 field, instead of
leaving it as None.

Operations on Existing Queries
You can perform a scaling of an existing query, or a scaling and algebraic addition of two queries, or an integration or
differentiation of a query.

By Operating on Existing Queries
1. Select Sample as “By Operating On Existing Queries”
2. Select the operation.
(Combine/Scale, Integrate or
Differentiate).
For Combine/Scale (shown):
3. Select the Query Item and the
set the Scale Factor if you want
to scale a single query - or Select both Query Items and set both Scale Factors if you want to scale and add
algebraically.
3. Click Create
Note, if integrate or differentiate is chosen, you will only need to choose the query to operate on.

Queries From External Sources
You can import previously created and saved (or externally generated) EnSight queries or Dytran time history (.ths)
files.

Read From An External File
1. Select Sample as “Read From
An External File”.
2. Click the “Load XY Data From
File ...” button to open the File
Selection dialog, and select any
previously saved EnSight XY data
file or a Dytran .ths file.

Read from server file
You can ask the server for any queries that it knows about. Some data formats (acessed by user-defined readers)
have such. If any are available, they will show up in the list of Queries.

Page 303

Plotting
Once Queries exist, they can be easily plotted in a new plotter in EnSight, or if an existing plotter of the correct type
exists, they can be added to the existing plotter.
1. Select the Query Item to be
plotted.
2. Click the New Plotter button if a
new plotter is desired.
In this case we did not choose to plot
the displacement vs. Time query on
the already existing Maximum plastic
vs. Time plot. Instead we created a
new plotter.
3. Select the next Query Item to be plotted.
4. Select the existing plotter on
which to add this query plot.
In this case, the Minimum plastic vs.
Time query is added to the existing
plot for Maximum plastic vs. Time ) thus the plotter will now have two
curves on it.

Note: the toggle indicated controls whether the plot is automatically rescaled
whenever a curve is assigned to it, or not.

OTHER NOTES
See XY Plot Data Format in the User Manual for a description of the plot file format.

SEE ALSO
How To Probe Interactively
How To Change Plot Attributes
User Manual: Query/Plot

Page 304

Change Plot Attributes

INTRODUCTION
EnSight provides a full-featured X-Y plotting system fully integrated with the query and transient data handling
capabilities. Query entities (see How To Query/Plot) are assigned to plotters. Plotters display one or more curves
where each curve is based on the data from a single query entity. If the query entity is changed, the corresponding
curve will automatically update. Plotter attributes (controlling aspects of appearance such as color of curves and
titles, axis labeling, gradation and tick marks, and border/background color) can be edited in Plot Mode.
This article is divided into the following sections:
Anatomy of a Plotter
Create Plotters
Select Plotters and Curves
Move and Resize Plotters
Set Plotter Visibility
Set Title, Background, Legend, Border, Position, Time Attributes
Set Axis Attributes
Set Curve Attributes
Delete Plotters

Anatomy of a Plotter
Plotters are composed of the following fundamental components:
Plot Title
Plot Scale Handle (grab to
scale all except Plot Title
and Legend)

Y Axis Value Labels

Y Axis Gradation

Legend
Legend Position Handle

Y Axis Subgradation

Y Axis Title
Curves

X Axis Value Labels
Plot border (red indicates
that it is currently selected)
X Axis Title

Page 305

Create Plotters
Plotters are automatically created when you assign a query entity to a new plotter (see How To Query/Plot for
details).

Select Plotters and Curves
When you create a new plotter, it automatically becomes the currently selected plotter (as shown by the border drawn
in the default highlight color). Any action to change plotter attributes always operates on the currently selected
plotter(s) (or the plotter defaults if none are selected). To select plotters:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Move the mouse pointer into the Graphics Window and click the left mouse button anywhere within
the desired plotter. You can add to an existing selection by holding down the Control key as you click
in additional plotters.
Since plotters may contain multiple curves, it is necessary to select individual curves within a plotter for subsequent
action. If no curves are selected, changes to curve attributes reset the defaults for subsequently created curves. To
select curves within a plotter:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Move the mouse pointer into the graphics window and click the left mouse button on the desired
curve. You can add to an existing selection by holding down the Control key as you click on
additional curves.

Move and Resize Plotters
Plotters can be easily moved and resized. You can either reposition a plotter with the mouse in the Graphics Window,
or precisely by entering exact values. To move or resize a plotter interactively:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired plotter (as described above).
3. To move a plotter, move the mouse pointer into the Graphics Window and into the selected plotter.
Click and hold the left mouse button and drag the plotter to the desired location.
4. To resize a plotter, move the mouse pointer into the Graphics Window and place the it over one corner
or side of the selected plotter. Click and hold the left mouse button and drag the corner or side to the
desired location.
A plotter can also be positioned precisely. See below for details.

Set Plotter Visibility
Selected plotters can be made invisible:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired plotter(s).
3. Click the Plotter Visibility Toggle to toggle display of the
selected plotters on or off (when not in Plot Mode).

Off

On

Plotters that are currently invisible are displayed dimmed while in Plot mode.

Page 306

Set Title, Background, Legend, Border, Position, Time Attributes
Overall attributes of plotters are controlled through the Plotter Specific Attributes dialog:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired plotter(s).
3. Click the Graph Attributes icon.

The Plotter Specific Attributes dialog contains six sections: Background, Border, Legend, Position, Time, and Title.
Click the tab at the top to display the corresponding section.
The Background section controls the type and color of the plotter background:

Set background type to either None or Solid.
A solid background is opaque.
If the background type is Solid, set the color
(either enter new values in the RGB fields or
click the Mix... button to open the Color
Selector dialog).

The Border section controls the visibility and color of the plotter border:

Toggle border visibility
Set border color (either enter new values in
the RGB fields or click the Mix... button to
open the Color Selector dialog)

The Legend section controls the plotter legend text. The actual text in the legend is specific to the individual curves
displayed in the plotter. See Set Curve Attributes below.

Toggle legend visibility
Set text size
Set origin (with respect to lower left corner
of plotter)
Set text color (either enter new values in the
RGB fields or click the Mix... button to open
the Color Selector dialog)

Page 307

The Position section controls the size and position of the plotter:
Set the origin of the plotter (with respect to
the lower left corner of the Graphics
Window).
Set the plotter width/height (0-1 normalized
to the width and height of the Graphics
WIndow)

The Time section controls whether the curves will animate and whether the plot will be swept out during the animation
or whether a time marker will sweep along the curve in the plotter:

Select Animate curves if you want the curve
to be swept out or a time marker to be swept
along the curve during animation.
Toggle Display time marker on if you want a
vertical line to sweep along the curve during
animation. Otherwise the curve itself will be
swept as animation proceeds.
You can control the line width, style, and
color of a time marker.

The Title section controls the main title at the top of the plotter (remember to press return after changing a text field):

Set title text
Set the size of the title text
Set the text color (either enter new values in
the RGB fields or click the Mix... button to
open the Color Selector dialog)
If you desire special symbols, click Insert
Symbol, pick the symbol(s), close, then hit
return in the title field.

Page 308

Set Axis Attributes
Axis attributes of plotters are controlled through the Axis Specific Attributes dialog:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired plotter(s).
3. Click the Axis Attributes icon.

The Axis Specific Attributes dialog contains three sections: General, X-Axis, and Y-Axis. Click the button at the top to
display the corresponding section.
The General section controls axis width, color, and scaling as well as Gradation and Subgradation marks.

Set line width of axes
Set color of axes
Set auto scaling - when on, the Min/Max values and the
number of gradations (attributes for the X-Axis and Y-Axis) will
be used as suggested values to arrive at pleasing numbers for
the axis labels.
Set line width, style, and color for major gradations (gradations
are enabled on a per-axis basis in the X-Axis and Y-Axis
sections)
Set line width, style, and color for subgradations
(subgradations are enabled on a per-axis basis in the X-Axis
and Y-Axis sections)

Page 309

The X/Y-Axis section controls the title, value labels, and gradation marks for the X or Y axis.

Choose which axis to deal with
Toggle visibility of the axis line
Set the origin location of the plot (with respect to the left/
bottom edge of the plotter)
Set the width/height of the plot (with respect to the width/
height of the plotter)
Set the title of the axis
Set the size of the title of the axis
Set the color of the title of the axis
Set the type of axis label: None (show no value labels), All
(show value labels at each gradation), or Beg/End (show
only the first and last value labels)
Set the size of the axis value labels
Set the scale to linear or logarithmic(log10)
Set the min/max range of the variable displayed on the axis
(Note: will be used as exact values only if the Auto Axis
Scaling toggle under the General Section is off.)
Set the display format of the value labels (or click Format...
to select common formats from a list)
Set the color of the axis value labels
Set the type of gradation: None (no gradation marker), Grid
(a vertical line), or Tick (a mark on the axis at the value label
positions)
Set the approximate number of gradations (also depends on
the min/max range)
Set the type of subgradation: None (no subgradation
marker), Grid (a vertical line), or Tick (marks on the axis
between the value label positions)
Set the number of subgradations between each value label
By swapping the min and max can swap the positive
direction.

Page 310

Set Curve Attributes
Curve attributes are controlled through the Curve Specific Attributes dialog:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired curve(s) by clicking on them in the
Graphics Window (control-click to select multiple curves).
If no curves are selected, any changes are applied to the curve
defaults which will effect any curves created in the future.
3. Click the Curve Attributes icon.
Set the description text for the curve (this will appear as the
legend)
If desired, you can apply scale factors to your x and/or y data
Set the line width
Set the line style
Set the line type:
None (only curve markers are drawn),
Connect Dots (data points are connected by straight lines),
Smooth (a piece wise spline is fit to the data points using the
number of points specified in the Smooth Sub-points field)
Set the marker type
Set the size of the markers
Normalize x and/or y values, if desired.
Set the color of the curve

Delete Plotters
Existing plotters can be deleted:
1. Click Plot in the Mode Selection area to enter Plot mode.
2. Select the desired plotter(s).
3. Click the Delete icon.

Note that deleting a plotter
has no effect on any query
entities that were attached
to the plotter

Select All
You can select all curves or all plotters.

Page 311

SEE ALSO
How To Query/Plot
User Manual: Plot Mode

Page 312

Query Datasets

INTRODUCTION
Results datasets often consist of multiple files. EnSight provides a mechanism to quickly ascertain basic information
about dataset files.

BASIC OPERATION
To display dataset information:
1. Select Query > Dataset...

The Associated Files section displays all
dataset files giving the size in bytes and
last modification date.

The File Specific Information section
displays information about the file
currently selected in the Associated Files
list. The information presented varies
based on the file type and format.
The General Geometric section displays
whether the geometry is static (time
invariant), changing coordinates (nodal
coordinates update each timestep), or
changing connectivity (coordinates plus
connectivity update every timestep).
Further the 3D extent of all geometry as
well as the number of nodes and elements
is displayed.

The Element Detail section shows the
type and number of all unique element
types in the dataset.

SEE ALSO
User Manual: Query Dataset

Page 313

Manipulate Parts
Change Color

INTRODUCTION
In EnSight, parts can be colored either by a constant color or based on the value of a variable. Coloring geometry by
variables is one of the simplest and most effective means of visualizing the distribution of a variable.
You can also set a “default” color – all parts subsequently created will automatically be colored by the default color
(described in the Other Notes section below).
This article covers changing the color of a part. See How To Edit Color Maps for information on changing the
mapping from variable values to color.

BASIC OPERATION
To change a part’s color:
1. Select the desired
part(s) in the Main
Parts List.
2. Click the Color
icon.
Which will open the
Part Color dialog.

3. If coloring by a variable,
select the variable in the
‘Color by’ pulldown.
4. If coloring by a vector
component turn on the Show
components toggle.

5. If coloring by a constant color, select a color
from the color matrix.
- OR 6. click the More... area to open the Color Selector
dialog

Page 314

OTHER NOTES
If coloring by a nodal variable, the default coloring will be continuously varying - even within a given element. If you
are coloring by a per-element variable, the coloring will not vary within a given element. If you desire to see perelement variables in a continuously varying manner, you can toggle on “Use continuous palette for per element vars”
under Edit->Preferences... Color Palettes. .
You can set a default variable that will be used to color all
subsequently created parts. To do this, be sure no parts are
selected in the Main Parts list. (To de-select a part, hold down
the control key as you click on the selected item.)
Select the desired default variable in the Variables list of the
Part color, lighting, & transparency dialog as described in 3. and
4. above.
Any part created subsequently will automatically be colored by
the default variable.
Applying 2D Textures:
You can also apply 2D textures to a part, by clicking the Edit
texture.. button here. The Textures dialog will be opened.
See How To Map Textures

SEE ALSO
How To Edit Color Maps.
How To Map Textures
User Manual: Color Selector

Page 315

Copy a Part

INTRODUCTION
The copy operation creates a dependent shallow (only on client) copy of another part. The new part has its own set
of attributes (except for representation), but shares geometric and variable data with the original. One of the best
reasons to create a copy is to show multiple variables on one part at the same time in a side-by-side configuration.
The copy can be moved independently since new copies are automatically assigned a new frame.

BASIC OPERATION
To create a copy of a part or parts:
1. Select the desired part(s) in the Parts List. A separate copy will be created for each selected part.
2. Select Edit > Part > Copy.
2. OR, just right click on the part
name in the part list and choose
‘Copy’.

The new copies will be added to the end of the Parts List with “– COPY” appended to the part description.

ADVANCED USAGE
The most common reason for needing a copy of a part is to display multiple variables on the same geometry
simultaneously. When you create a copy, a new Frame is also created and the copy is assigned to it (when you
create multiple copies at the same time, a new frame is created for each new copy). Using Frame Mode, frames can
be manipulated (e.g. translated or rotated) independently. See How To Create and Manipulate Frames for more
information.

OTHER NOTES
The dependence of the copy on the original has some important consequences:
1. If you change the visual representation of the original, the representation of the copy will change as well.
2. You cannot delete the original until the copy has also been deleted.
3. Since the part copy only exists on the client, you cannot save a part copy to disk.
If you want to create a dependent, non-shallow copy of a part, you can perform a merge operation on a single part.
This type of copy does now have the same consequences: the resulting “copy” is basically independent except that it
cannot exist without its parent.

SEE ALSO
User Manual: Part Operations

Page 316

Group Parts

INTRODUCTION
In many types of analysis, multiple parts are used to distinguish between various components or material types. To
the extent allowed by the particular data format, EnSight maintains this distinction by assigning these entities to
separate model parts. In many cases however, this distinction is no longer useful for postprocessing. When
manipulating parts, you often need to apply the same set of attributes to all of them. If the number of parts to be
treated identically is large, this process can become unwieldy. EnSight provides a group operator to combine multiple
parts of the same type and case into a single part. The selected parts for the group are automatically removed from
the user interface, leaving only the newly formed group part. The operation can be reversed by performing the
Ungroup command.

BASIC OPERATION
1. Select the desired part(s) in the Parts List.

2. Select Edit > Part > Group
(or right click in the part list)
2. OR right click on the part name
in the part list and choose
‘Group...’

3. Enter a new part name in the
pop-up dialog.

The selected parts for the group are removed from the part list, and a new Group part is added to the end of the Parts
List.

OTHER NOTES
The operation can be reversed by selecting Edit > Part > Ungroup (or right click on the group name in the part list and
choose ‘Ungroup’.
Grouped parts cannot contain other grouped parts.

SEE ALSO
User Manual: “Part Operations”

Page 317

Merge Parts

INTRODUCTION
In many types of analysis, multiple parts are used to distinguish between various components or material types. To
the extent allowed by the particular data format, EnSight maintains this distinction by assigning these entities to
separate model parts. In many cases however, this distinction is no longer useful for postprocessing. When
manipulating parts, you often need to apply the same set of attributes to all of them. If the number of parts to be
treated identically is large, this process can become unwieldy. EnSight provides a merge operator to combine
multiple parts into a single part.
The merge operation creates one new part from one or more selected parent parts. The original parts are
unchanged. If only a single part is selected for the operation, merge will create a “true” copy of the part (as opposed
to the shallow copy that the Copy operation creates), with the only dependence being that the parent must exist.
If you delete any of the original parts after the merge, these components will be deleted from the merged part as well.

BASIC OPERATION
1. Select the desired part(s) in the Parts List.

2. Select Edit > Part > Merge

The new merged part is added to the end of the Parts List with the description “Merge of parts #,#,#” where # are the
part numbers of the originally selected parts.

OTHER NOTES
Unlike Copy, merge creates true, server-based parts. Unlike Extract, merge creates parts based on the full, serverbased representation of the part.
If you merge a structured (IJK) part, the resulting part will be unstructured.

SEE ALSO
How To Group Parts.
User Manual: “Part Operations”

Page 318

Extract Part Representations

INTRODUCTION
The extract operation is closely tied to part representations. Extract creates a single new part using only the
geometry of the current representation of the selected part(s). For example, if the current representation of a part
consisting of 3D elements is Border, the result of extraction will be a part consisting of all unshared 2D elements (the
surface).
Extract is most often used to reduce the amount of information for a part (e.g. for faster display or for geometry
output) or to create a surface shell part – perhaps for subsequent cutting – of a 3D computational domain.

BASIC OPERATION
1. Select the desired part(s) in the Parts List.

2. Select Edit > Part > Extract

The new part is added to the end of the Parts List with the description “Extract of parts #,#,#” where # are the part
numbers of the originally selected parts.

SEE ALSO
See How To Change Visual Representation.
User Manual: “Part Operations”

Page 319

Cut Parts

INTRODUCTION
It is sometimes desirable to cut parts to, for example, reveal the interior of a solid or remove unwanted or unneeded
portions of a model. EnSight can cut any server-based part and either keep both “sides” or discard one. Any of the 3D
tools (Plane, Quadric, or Box) can be used as the cutting surface.
The cut operation produces dependent copies of the parent part. The part(s) resulting from a cut are completely valid
parts consisting of standard element types. These parts can be used for any operation – including further cuts.

BASIC OPERATION
To cut a part:
1. Select the part(s) in the Main Parts list.
2. Click the Clip Feature icon.
3. Select the desired cutting tool (Plane, Box,
Cylinder, Sphere, Cone, Surface of
Revolution or Revolve 1D Part).
4. Position the desired cutting tool in the
desired location.
5. Select which “sides” to keep.
.

Inside: Keeps inside of quadrics or box and “front” of plane.
Outside: Keeps outside of quadrics or box and “back” of plane.
In/Out: Keeps both sides

Crinkly: Keeps all elements that intersect the plane.
For the Plane tool, the inside is the positive Z side of the tool. For the quadric tools, the inside and outside are
intuitive. In the Main Parts list, the original part remains and cannot be deleted without also deleting the cut parts (but
can easily be made invisible if desired). If In/Out was used, two new parts are added to the end of the Main Parts list
with the same name as the original part with “+” added to the name of the Inside part and “–” appended to the name
of the Outside part. If Inside or Outside was used, one new part is created with “+” added to the beginning of the
name.

OTHER NOTES
A part copy cannot be cut. However, if the parent of the copy is cut, the copy will be cut as well (since part copies
share geometry with the parent).
The cut operation maintains the order of the elements, e.g. 3D elements yield 3D elements and 3D quadric elements
yield 3D quadric elements.
The cut algorithm breaks elements intersecting the cutting surface into tetrahedrons. Since there is no transition
zone created between these tetrahedrons and their non-cut neighbors, non-shared element faces are possible.
These non-shared faces can result in undesired lines and/or elements during border and/or feature angle
representations.
If you cut a structured (IJK) part the resulting parts will be unstructured.
Cuts with the Box are not true cuts, but simply a division of all elements that fall completely within the box or not.

SEE ALSO
User Manual: Part Operations

Page 320

Delete a Part

INTRODUCTION
The delete operation removes selected parts and any parts dependent on them. All information associated with the
parts on both the client and server is removed. Deletion cannot be undone.

BASIC OPERATION
1. Select the desired part(s) in the Parts List.

2. Select Edit > Part > Delete
or click the Delete... button
below the main parts list
or click the Delete key on your
keyboard while the mouse is
in the EnSight window
or right click and select
Delete.

3. Confirm the deletion.

OTHER NOTES
In some cases, variables that depend on a deleted part may have to be updated. For example, if you have a variable
such as Area calculated on a set of parts and one of the parts is deleted, the Area variable will automatically be
recalculated.
If you delete a grouped part, all parts in the group will be deleted.

SEE ALSO
User Manual: “Part Operations”

Page 321

Change the Visual Representation

INTRODUCTION
The ability to change part representations is a powerful management tool in EnSight. Not only can you select the
visual representation that best meets your needs, you can also manage memory more effectively. Part
representations exist on the client, the full part is maintained by the server. Using simpler representations both
reduces your client memory consumption as well as improving graphics display speed.
EnSight provides five representation modes for parts (as well as three modes that are a combination of the five
depending on the dimensional order of parts):
Full
Border

Every face and edge of every element is displayed.
Only unshared faces (for 3D parts) or unshared edges (for 2D parts) are
displayed.

3D Border, 2D Full

Display 3D parts in Border representation; display 2D parts in Full
representation.

3D Feature, 2D Full

Display 3D parts in Feature representation; display 2D parts in Full
representation.

3D nonvisual, 2D Full

Display 3D parts in Non Visual representation; display 2D parts in Full
representation.

Feature Angle

Only those edges joining faces in the Border representation for which the
angle between the faces is less than some threshold are displayed.
Feature Angle typically extracts the topological features of interest in a
model.

Bounding Box

Only a wireframe box representing the XYZ extents is displayed.

Non Visual

No visual representation exists on the client. It is often useful to use Non
Visual as the representation for 3D computational domain parts –
provided you also have some sort of shell part to display the outer
surface.

Volume

Every element is displayed with a controllable level of transparency. Use
this with caution as this can require a large amount of memory on your
hardware graphics card.

Additionally, one can specify that only a point and normal (instead of the element connectivity) for the specified
representation be loaded. This is most useful for very dense models.
The sitewide default visual representation (as well as extension mapping) is individually specified for data formats in
the $CEI_HOME/ensight92/site_preferences/ensight_reader_extension.map file. For example
.case files always open with the EnSight Case gold reader and parts are always in 3D Feature, 2D Full mode.
Custom visual representation can be specified in the user’s local ensight_reader_extension.map file located in
the users local EnSight Defaults directory.

Page 322

BASIC OPERATION
1. Select the desired part(s) in the Parts List.
2. Select Part in the Mode Selection area to enter
Part mode.
3. Click the Element Representation icon to open
the Part Element Settings dialog.
4. Select the desired visual representation.
Options are:

5. If desired, you can have each element
connectivity of your element representation be
replaced by a point and normal only.
6. If desired, you can apply polygon reduction.
Polygon reduction is designed to speed up visualization
processing by thinning out the number of polygons that are
rendered. There is naturally a trade off in image quality and
speed. Note that the original model is not modified, just its
rendered image.

OTHER NOTES
Note that some derived parts (such as contours or vector arrows) are based on the client’s representation of the
parent part. If the parent’s representation changes, the derived parts will change as well.
You cannot change the representation of a copied part. A copy always exhibits the current representation of the
original part.
A part’s representation can be made “permanent” by creating a new part based on the current representation. See
How to Extract Part Representations for more information.

SEE ALSO
User Manual: Element Representation

Page 323

Set Attributes

INTRODUCTION
Part attributes control the appearance and behavior of parts. Much of the power of EnSight derives from the broad
range of attributes available and the ease with which they can be changed. Attributes are grouped into several
classes:
Creation

Creation attributes are unique for each (non-model) part type (e.g. the isovalue of an isosurface). Most (if
not all) of the creation attributes for a part are accessible in the Quick Interaction area after doubleclicking the part in the Main Parts List, or by the main menu structure Edit->Part Feature Detail Editors>Isosurfaces (for example). A model part attribute controlling whether the given mesh elements will be
used, or whether the model nodes will be used to create a new 2D or 3D mesh is available in this section.

General

Visibility
Susceptibility to auxiliary clipping
Reference Frame
Response to change in time (active or frozen)
Symmetry options
Viewport visibility
Coloration (by variable or constant color)
Hidden surface toggle
Hidden line toggle
Shading type (flat, Gouraud, smooth)
Transparency
Lighting (diffuse, shininess, highlight intensity)
Visual symmetry

Node, Element,
and Line

Node, line, element visibility toggles
Node type (dot, cross, sphere)
Node scale (constant or variable)
Node detail (for spheres)
Node and element label toggle
Element-line width
Element-line style (solid, dotted, or dot-dash)
Element representation on client (full, border, 3D border/2D full, 3D feature/2D full, 3D nonvisual/2d full,
feature angle, bounding box, nonvisual)
Element shrink factor
Polygon reduction factor
Failed element variable and rules

Displacement

Displacement variable
Displacement scaling factor

IJK Axis Display

IJK Axis visibility
IJK Axis scale value

Most (if not all) of the Creation attributes for non-model parts can be edited in the Quick Interaction area by doubleclicking on the part in the Main Parts list. Most display attributes (such as color and visibility) can be controlled via the
icons in Part mode. If required, the Feature Detail Editor can be opened for complete access to all attributes. See
How To Use the Feature Detail Editors for more information.
Since Creation attributes are specific to each (non-model) part type, they are not covered here. Look in the How To
article for the specific part type for details on those particular Creation attributes.
Server side displacement capability is available in the Creation Attribute area for model parts. See How To Display
Displacements for a description of this capability.
This article is divided into the following sections:
Part Mode Attribute Icons
General Attributes
Node, Element, and Line Attributes
Displacement Attributes
IJK Axis Display Attributes

Page 324

BASIC OPERATION
Part Mode Attribute Icons
The Part mode icons can be used to quickly set attributes for parts. To use these controls:
1. Select the desired part(s) in the Main Parts list.
2. Click Part in the Mode Selection area.
3. Click appropriate icon to set the desired attribute:

Part Visibility
Color, Lighting, & transparency
Line Width
Visibility Per Viewport
Element Visual Representation
Displacement
Visual Symmetry
Node and Element Labeling
Node Representation
Failed Elements
Element Blanking
Shading Type
Hidden Line
Auxiliary Clipping
Fast Display Representation

Page 325

General Attributes
The General Attributes section in the Feature Detail Editor duplicates many of the controls available in Part mode. To
set attributes using the General Attributes section:
1. Right click on the part name in the part list and choose ‘Edit’ or right click on the part in
the graphics window and choose ‘Edit’.
1. OR Select Edit > Part Feature Detail Editors > part type.
2. In the parts list at the top of the Feature Detail Editor dialog, select the desired part(s).
By default, any changes you make to attributes will take effect immediately. If you wish to “batch” a
series of changes, select Edit >
Immediate Modification (be sure
to use the Edit menu in the
Feature Detail Editor dialog) to
toggle this setting off. When

Set part detail representation
(according to Global
Viewing Detail Mode):

Toggle part visibility
Toggle auxiliary clipping on/off
Toggle whether the client’s portion
of the part changes if the current
time step changes

• Box: part is represented as
bounding box.
• Elements: part is represented
according to Element
Representation
• Points: part is represented as
a point cloud
Set part reference frame

Set color by constant or color by
variable
Set the part color if constant

Set part graphical symmetry

Toggle part hidden surface

Set shading type:

Toggle part hidden line

• Flat: color and shading are
constant across elements

Set part transparency as “true”
or with a fill pattern

• Gouraud: color and shading
vary linearly across elements

Set part shading parameters:

• Smooth: color and shading
calculated based on surface
normal interpolated across
elements to simulate a
smooth surface.

• Diff: diffuse shading – the
amount of light that a surface
reflects. 0 is none and 1 is full.
• Shin: Degree of shininess – 0 is
dull and 100 is very shiny.
• H Int: Degree of highlight
intensity – 0 is none and 1 is full.

SEE ALSO
Set Global Viewing Parameters

Page 326

Node, Element, and Line Attributes
Node, element, and line attributes control how a part’s nodes and elements are displayed. Nodes can be displayed
as dots, crosses, or spheres. If displayed as crosses or spheres, the radius can be set by the value of a variable at
that node. To set attributes using the Node, Element, and Line Attributes section:
1. Select Edit > Part Feature Detail Editors > part type.
2. In the parts list at the top of the Feature Detail Editor dialog, select the desired part(s).
By default, any changes you make to attributes will take effect immediately. If you wish to “batch” a series of
changes, select Edit > Immediate Modification (be sure to use the Edit menu in the Feature Detail Editor dialog) to
toggle this setting off. When toggled off, a button at the bottom of the dialog becomes active: Apply Changes.
Click it when you are ready to apply a set of changes.
3. Set the desired attribute(s):

Set node representation
Set visibility of nodes, lines,
elements

• Dot: nodes are displayed as
points.

Set node/element label visibility

• Cross: nodes are displayed as
crosses and can be fixed size
(size set by the Scale value) or
sized based on a variable (and
scaled by the Scale value).

Set Line width and Style (Solid,
Dotted, or Dot-dashed)

• Sphere: nodes are displayed as
spheres and can be fixed size
(size set by the Scale value) or
sized based on a variable (and
scaled by the Scale value).
Sphere detail controlled by Detail
value.

Set element representation
(described below)
Set element shrink factor (shrink
elements toward the centroid)
Set angle for Feature Angle
representation

Set polygon reduction. Same
model, but simpler representation.
Trade-off of visual fidelity and
rendering speed.

Set variable to use for failed
element removal.
Set the values and rules for failed
element variable values

Page 327

EnSight provides five representation modes (and three combination modes) for parts (see also How To Change
Visual Representation):
Full
Border
3D Border, 2D Full
3D Feature, 2D Full
3D nonvisual, 2D Full
Feature Angle

Non Visual

Bounding Box

Every face and edge of every element is displayed.
Only unshared faces (for 3D parts) or unshared edges (for 2D parts) are displayed.
Display 3D parts in Border representation; display 2D parts in Full representation. This is the
default representation for all parts.
Display 3D parts in Feature representation; display 2D parts in Full representation.
Display 3D parts in Non Visual representation; display 2D parts in Full representation.
Only those edges joining faces in the Border representation for which the angle between the
faces is less than some threshold are displayed. Feature Angle typically extracts the
topological features of interest in a model.
No visual representation exists on the client. It is often useful to use Non Visual as the
representation for 3D computational domain parts – provided you also have some sort of shell
part to display the outer surface.
Displays a bounding box surrounding (and in place of) the nodes and elements.

Displacement Attributes
In structural mechanics simulations, a common output variable is a set of vectors representing the movement or
displacement of geometry. Each displacement vector specifies a translation of a node from its original position (an
offset). EnSight can display and animate these displacements to help visualize the relative motion of geometry. To set
Displacement attributes (see also How To Display Displacements):

Set Displace By to either None (no displacement) or the vector variable to
use for displacement.
Set nodal displacement factor to reduce or exaggerate a displacement

IJK Axis Display Attributes
Model Parts and clips (because they can be structured parts) will have these attributes available. These attributes will
only be applicable to structured parts.
Toggle IJK Axis Visible to display an IJK axis for the part.
The scale factor for the IJK Axis triad can be modified in this field.

SEE ALSO
Introduction to Part Creation
User Manual: Part Attributes
Page 328

Display Labels

INTRODUCTION
It is often useful to be able to identify specific nodes or elements within your model. EnSight can display node and
element labels in the Graphics Window. If your data provides explicit node or element labels (or you are using
EnSight data formats and have asked EnSight to assign ids), EnSight will be able to display those values. Only model
parts can have labels.
Displaying labels on parts with thousands of nodes or elements can obscure both the geometry as well as the labels
of interest (as well as degrading display performance). EnSight provides a filtering mechanism to display only
selected ranges of labels.

BASIC OPERATION
Displaying Node and/or Element Labels
To display labels (and to control filtering and coloring):
1. Select the desired part(s) in the Main Parts list.
2. Select Part mode in the Mode Selection area.
3. Click the Node/Element Label icon to display the Node/Element
labeling attributes dialog.

4. Click the appropriate
toggle(s) to turn on/off node
and/or element labels.
5. To set filters for node/
element labels, select the
desired filter and enter the
appropriate values in the
Low and/or High fields.
6. Set the node/element label
color.

The label filters operate as follows:
None

Display all labels.

Low

Remove all labels < the Low value

Band

Remove all labels >= Low and <= High

High

Remove all labels > the High value

Low/High

Remove all labels < the Low value as well as those > the High value.

Page 329

Note that the Node and Element Label toggles also have counterpart toggles in the View Menu. These act as global
toggles that enable or disable any per-part node or element labels.

OTHER NOTES
Note that created parts do not have node or element labels.
Note: The font size of the node and element labels can be modified under Edit > Preferences > Annotation. Simply
change the value in the 3D label size field and hit a return. If desired, this change can be made permanent for future
EnSight sessions by hitting the Save to preference file button.
Another useful technique for reducing label clutter is to use the front and back Z clipping planes to display only a thin
slice of interest. See How To Set Z Clipping for more information.

SEE ALSO
User Manual: Label Visibility

Page 330

Set Transparency

INTRODUCTION
EnSight can display parts as transparent using two different methods:
True (alpha)

Fill Pattern

True transparency uses the hardware alpha planes. Although the resulting visual effect is
superior to fill patterns, true transparency is slower to draw (especially for large models)
since multiple draw passes must be performed.
Fill pattern or screen-door transparency uses polygon fill patterns to provide a pseudotransparency effect. EnSight provides three patterns.

BASIC OPERATION
1. Select the desired part(s) in the Parts List.
2. Select Part in the Mode Selection area to enter
Part mode.

3. Click the Part color, lighting, & transparency
icon to open corresponding dialog.

For true transparency:
4. Adjust the slider to the desired
setting.
The Graphics Window will dynamically
update as the slider is adjusted.
OR
For Fill Pattern transparency:
4. Select the desired pattern from the
Fill Pattern pulldown.

SHORTCUT
Right click on the part of interest in the
graphics window and select ‘Color by >’
then ‘Variable’, ‘Color’, or choose ‘Make
Transparent’

SEE ALSO
User Manual: Part Transparency

Page 331

Select Parts

INTRODUCTION
Manipulating parts is one of the fundamental operations in EnSight. Before you operate on parts, they must be
selected in the Main Parts list. Parts can either be selected through standard mouse interaction with the items in the
Main Parts list or selected by picking parts in the Graphics window.

BASIC OPERATION
Selecting Parts in the Graphics Area
Left click on the part in the graphics window to select in the main part list. Use control key to select multiple parts.

Selecting Parts using the Main Parts List
Items in the Parts List itself are selected using standard Motif methods:
To ...

Do this ...

Details ...

Select an item

Select (or single-click)

Place the mouse pointer over the item and click the left mouse
button. The item is highlighted to reflect the “selected” state.

Extend a contiguous
selection

Select-drag

Place the mouse pointer over the first item. Click and hold the left
mouse button as you drag over the remaining items to be
selected. Only contiguous items may be selected in this fashion.

Extend a (possibly long)
contiguous selection

Shift-click

Select the first item. Place the mouse pointer over the last item in
the list to be selected. Press the shift key and click the left mouse
button. This action will extend a selection to include all those
items sequentially listed between the first selection and this one.

Extend a non-contiguous
selection

Control-click

Place the mouse pointer over the item. Press the control key and
click the left mouse button. This action will extend a selection by
adding the new item, but not those in-between any previously
selected items.

De-select an item

Control-click

Place the mouse pointer over the selected item. Press the control
key and click the left mouse button. This action will de-select the
item.

Open the Quick
Interaction Area for a part

Double-click

Place the mouse pointer over the item and click the left mouse
button twice in rapid succession.

Selecting Parts using the Select... Options
There are several other useful options for selecting parts:
1. Click the Select... button just below the main parts list.
2. Select the desired option.
All

Selects all parts in the list.

Invert

Inverts the selection. Namely, all parts currently
selected become unselected and all unselected
become selected.

Invisible

Selects all visible parts.

Visible

Selects all invisible parts

Region

Selects all parts that are within the selection tool.
(Requires that the selection tool be on)

Showing

Selects all visible parts which are showing in the
graphics window.

Keyword... Opens a dialog which allows for selections using
keywords and regular expressions.
Unselect

Unselects all parts in the list.

Page 332

Selecting Parts by Picking
Parts can also be selected by “picking” them in the Graphics window. To select parts by picking:
1. From the Pick pulldown icon, select Pick Part.
(Note that this is the default, and this setting will be retained
until explicitly changed.)
2. Position the mouse pointer over the desired part in the
Graphics Window and press the ‘p’ key (or perform the
mouse action which has been set to “Selected pick action”
in Edit > Preferences > Mouse and Keyboard).
See below regarding how parts are identified.
Note that the picked part is now selected in the Main Parts list.

Parts are identified for picking as follows. If the part (as represented on the client) consists of surface (2D) elements,
a pick will occur if the mouse cursor is over any portion of the surface – even if the part is drawn in line mode and the
mouse was over the middle of the element (and not over one of the visible lines). If the part is drawn as 1D elements
(e.g. the part is in feature angle representation), the mouse must be over one of the visible lines of the part.
By default, when you press the ‘p’ key any previously selected parts are de-selected. Holding down the Control key
as you hit ‘p’ modifies this behavior: if the picked part is not currently selected, it will be added to the existing selection
(so you can select multiple parts by picking), otherwise the picked part is de-selected.

Page 333

OTHER NOTES

1. By default, parts selected in the
part list are shown highlighted.

2. A global toggle turns this on
(default) and off
To turn this off permanently,
simply toggle it off and then
open Edit->Preferences->View
and press the "Save to
preferences file" button.

3. Unselected parts are shown
normal

SEE ALSO
User Manual: “Part Selection and Identification”

Page 334

Set Symmetry

INTRODUCTION
In many instances, a modeler can take advantage of symmetry present in a problem to reduce the computational
complexity of a subsequent analysis. EnSight can impart visual realism to such models by mirroring parts around any
or all axes of the part’s reference frame or performing rotational symmetry about any of the axes. Although the
mirrored or rotated portions appear identical to the source part (except for the reflection or rotation), they are only
visual (client-based) and cannot be used for calculation. For example, you cannot start a particle trace in one half
and expect the trace to cross the plane of symmetry into the other half (although you can make the particle trace part
symmetric as well).
EnSight also provides “true” or “computational” symmetry operations (mirror, rotational, translational) as an attribute
of the part’s reference frame. With computational symmetry, you can trace particles across a periodic boundary.
Both types of symmetry (visual or computational) are based on the part’s reference frame. Although you can use
simple visual or computational symmetry without having to manipulate the frame, more advanced usage of symmetry
could require a working knowledge of frames. See How To Create and Manipulate Frames for more information.

BASIC OPERATION
Visual Symmetry
Visual symmetry is an attribute of parts. You can enable display of a mirrored copy of a part into one or more of the
seven octants (opposite of +,+,+) of the part’s reference frame. You can also enable display of a number of rotational
instances about the x,y, or z axes of the part’s reference frame. To display visual symmetry:
1. Select the desired part(s) in the Main Parts list.
2. Click Part in the Mode Selection area to enter Part mode.
3. Click the Visual Symmetry icon.

Visual Mirror Symmetry:
4. Select Mirror from the Type pulldown menu.
5. Select the desired octant(s) from the menu.

Visual Rotational Symmetry:
4. Select Rotational from the Type
pulldown menu.
5. Select rotational axis, instance
angle, and number of instances.

Recall that symmetry is performed with respect to the reference frame of the part. The frame’s axes define the
partitioning of space into the octants that attached parts are mirrored into, or the rotational axis. If the symmetry
operation did not produce the desired effect, it is probably due to the fact that the part’s frame is not aligned with the
plane of symmetry, or the rotational symmetry axis, as designed for the model. The solution is to create a new frame,
assign the part(s) to the new frame, and position the frame such that two of its axes lie in the plane of symmetry, or
one of its axes align with the rotational axis. There operations are discussed in How To Create and Manipulate
Frames.

Page 335

Computational Symmetry
Computational symmetry can be used for unstructured and structured model parts with periodic boundary conditions.
(Note, it does not work for created parts.) Computational symmetry can handle rotational, translational, and mirror
symmetry. Unlike visual symmetry, computational symmetry actually produces the symmetric geometry and variables
on the server - allowing for more than just visual symmetry.
You enable computational symmetry by selecting the frame, specifying the type (Mirror, Translational, Rotational),
and setting type specific attributes (such as the rotation angle and the number of instances to create). Each part
assigned to the frame will be updated on the server to reflect the specified symmetry.
Note that each new instance of a part created through computational symmetry creates a new part on the server.
To use computational symmetry, you will need to enable Frame Mode if it isn’t already enabled. (Edit > Preferences...
General User Interface - Frame Mode Allowed). Then:
1. Click Frame in the Mode Selection area to enter Frame mode.
2. If the default frame (frame 0) is not correctly positioned for the desired
symmetry operation, create a new frame, position the frame in the
proper location and orientation, and assign the part(s) to the new frame.
(See How To Create and Manipulate Frames for details.)
3. Select the desired frame.
4. Click the Computational Symmetry Attributes Icon.
The remaining steps depend on the type of symmetry desired.
Mirror Symmetry is similar to graphical symmetry as
described above.
5. Select Mirror from the Type pulldown.
6. Select the desired octant(s) from the Mirror In
pulldown.
7. Click Update.
Rotational Symmetry creates instances by rotating,
around the selected axis of the frame, the specified
number of degrees. The selected frame’s axis must
be aligned with the desired symmetry axis.
5. Select Rotational from the Type pulldown.
6. Select the frame rotational axis.
7. Set the desired rotation angle (in degrees) in
the Angle field.
8. Set the desired number of instances in the
Instances field (number 1 is the original, set
Instances to 2 to yield one copy).
9. If a periodic match file is available, toggle Use
Periodic File and enter the file name.
Periodic match files are discussed below.
10. Click Update.

Page 336

Translational Symmetry creates instances in the
direction of the specified translation vector. The
translation vector is first rotated by the frame’s
rotation, but is independent of the frame’s origin
location.
5. Select Translational from the Type pulldown.
6. Enter the desired translation vector in the XYZ
fields and press return.
7. Set the desired number of instances in the
Instances field (number 1 is the original, set
Instances to 2 to yield one copy).
8. If a periodic match file is available, toggle Use
Periodic File and enter the file name.
Periodic match files are discussed below.
9. Click Update.

Periodic Matching for Computational Symmetry
When a model is created with periodic boundary conditions, there is typically a built-in correspondence or “match”
between certain nodes and elements. For example:
7

The elements defined by nodes 1,2,3 and nodes 1,6,7 should
match when rotated about an axis passing through node 1
(perpendicular to the screen). When another instance is
created, node 2 matches with 6 and node 3 matches with 7.

5
6
4

3
2

1

When instances are added to a part, it is desirable to eliminate these duplicate nodes. Without a match file, EnSight
will attempt to find and remove them using a hashing scheme. This method works quite well, but may not find all
duplicates. (Remaining duplicates are usually noticed when the part is in feature angle representation since EnSight
treats elements with duplicate nodes as separate – even if they are coincident.)
Note that if you have a periodic match file you do not need to specify the rotation axis and angle in the Frame
Computational Symmetry Attributes dialog – the value is provided in the file.
A user-supplied matching file can be used to quickly find and remove all duplicates. The match file is a simple ASCII
text file. The file for the example above would be (the text in italics is not part of the file):
rotate_z
52.34
3
11
26
37

specifies rotational symmetry and the applicable axis
the angle of rotation (in degrees)
the number of node pairs to follow
first node pair
second node pair ...

See Periodic Match File for more information on periodic match files.

SEE ALSO
How To Create and Manipulate Frames

Page 337

Map Textures

INTRODUCTION
Texture mapping is a mechanism for placing an image on a surface or modulating the colors of a surface by various
manipulations of the pixels via a texture map image. EnSight supports the application of a texture onto a part and the
combining of texture effects with the normal EnSight coloring schemes. This can include animated textures(e.g. EVO
or MPEG files), which can be used to texture parts and 2D annotations.
The simplest use is to place a "decal"/logo or photograph on the surface of a part. Texturing can also be used to add
repeated patterns, provide custom transparency and lighting, color a part by multiple variables and clip parts to
arbitrary boundaries. A texture operation in EnSight consists of a texture map image, a collection of interpolation and
blending options and a mechanism for projecting the texture map image onto a part. Each of these items is described
in the following sections.
EnSight texture mapping is controlled through the "Textures" dialog, accessed through the 'Edit textures…' button in
the 'Part Color, Lighting and Transparency' dialog.

Setting the Texture
Map Image

Texture Operations
and Parameters

Texture Projections

Page 338

Setting the texture map image
EnSight supports up to 8 different textures, which are displayed as
thumbnails at the top of the dialog.

A number of operations can be
performed on the textures by rightclicking on the thumbnail image and
selecting from the menu.
A new image or movie (e.g. EVO,
MPEG, etc.) can be set for the texture
using the 'Load texture file…' option.
A texture can be reverted back to the
16x16 transparent checkerboard
default pattern using the 'Clear texture'
menu.
Each texture has a border color that is
used for colors outside of the texture
bounds. This color (RGB and opacity)
can be set explicitly using the 'Set
border color…' menu.

The eight textures are numbered one
through eight. Each part in EnSight can
have one of the eight texture
associated with it. This can be done by
selecting the part(s) and either clicking
on the appropriate button thumbnail or
selecting the number from the 'Use
texture' option menu.

Advanced options for loaded texture
images and animations can be set
using the ‘Set texture options...’
menu.
The basic information for the currently
selected texture is displayed in the text
field below the thumbnails. The size of
the texture, its source, border color and
the nature of its transparency (A channel
and border color) is displayed.

All textures have both a color (RGB) and an opacity (A) component. By default, the thumbnail
is drawn using the full RGBA pixel value. Options at the bottom of the menu allow the user to
select which channels to draw.
The lower row of images in the example dialog above are all the same texture, but drawn with a
different function.
The leftmost image is the full RGBA image,
the middle one is just the RGB part of the image
and the rightmost one is just the A part of the image.
Notice how the A channel masks out the black and white pixels in the RGB image. This masking can
be used to place non-rectangular images/icons on EnSight parts.
Users often make use of a common set of textures for many different analyses (e.g. company logos,
standard palettes, etc). The 'Save Default Textures' button allows the user to save the currently
loaded selection of textures and their display mode into the user's preferences directory. These will be
automatically loaded every time EnSight is launched.

Page 339

Setting Texture Options
In Ensight, animated textures (e.g. EVO or MPEG files)
can be used to texture parts and 2D annotations. Each
animated texture is linked to the current solution time in
EnSight. This temporal mapping can be set using the
“Texture options” dialog, selected from the button popup
menu.
Basic information about the texture is presented in the
upper pane.
This includes the filename, border color, dimensions, and
number of frames in the texture. It also includes temporal
reference information for animated textures.
Animated textures have a start and ending frame number.
These can be used to “crop” the texture to some subset of
the animation.
There is also a starting and ending solution time for the
texture.
The frame from the texture is selected such that the
starting frame number is used when the current EnSight
solution time is at or before the texture start time and the
ending frame is used when the current solution time is at
or after the ending time. The temporal mapping is linear
in-between.
There is also an “Autoscale” option.
If this option is set, the starting and ending time for that
texture will always be set to the dynamic range of currently
loaded EnSight solution times.
Note: EnSight will read the entire animation into memory
when it is loaded. If the movie is large, it can use a
significant amount of memory. In memory, EnSight uses
lossless compression schemes for the data. The current
scheme can be changed using the ‘Compression’ options
pulldown.
Since EnSight stores the entire animation in any exported
.els file, it can be advantageous to select and RLE or GZIP
compression scheme for large animations. In general, it is
suggested that users crop and resample movie files before
loading them as animated textures in EnSight.

Page 340

Texture operations and parameters
The interpolation scheme, repeat mode and texture mode define how textures are accessed and how they are
integrated into the normal EnSight coloring scheme.

The interpolation scheme can be linear or nearest. When the graphics hardware needs to
access a pixel in the current texture it will either use bilinear interpolation scheme or nearest
neighbor based on the setting for this item. Generally, linear results in smoother looking
displays, but can result in "fringes" that are the result of interpolating to colors that might not
exist in the native texture. Linear can be slower, but in EnSight, this is often the result of the fact
that a part may be turned translucent and need to be sorted during rendering (See Texture
implementation limitations). For applications where the exact colors in a texture are required,
the nearest neighbor interpolation method should be used.
EnSight allows the user to control the "repeat" mode for textures. When the current texture
projection specifies texture coordinates outside of the texture [0,1], EnSight can either "repeat"
the coordinates (e.g. a texture coordinate of 2.3 is mapped to 0.3) or it can "clamp" to the
border color of the texture. If repeat mode is set to repeat, the border color of the texture is not
used. Clamping is often used for logos and explicit texture coordinates (see Texture
projections).
The texture mode determines how a texture is combined with the natural coloring scheme in
EnSight. It has three values: "Replace", "Decal" and "Modulate". In replace mode, the base
colors provided by EnSight are ignored and the texture is used as the only source of color for
the part (note, this has the side effect of disabling any lighting). In decal mode, the alpha
channel of the texture is used to select between the texture color and the base color of the part.
If the texture alpha value is 0, the base color of the part is displayed, while locations where the
texture alpha value is 255, the texture color will be used exclusively. All alpha values inbetween 0 and 255 will result in an interpolation between the texture and base colors. Note that
the default texture uses an alpha channel with values 255 and 80. In modulate mode, the base
color is multiplied by the texture color and the resulting texture is used. Modulate mode is
commonly used with a texture that has a color of white and some pattern in the alpha channel.
This allows the base color to show through, but varies the transparency of the part. Arbitrary
clipping operations can be set up this way. Modulation of the color channels can be confusing
as the operation tends to suppress colors, but it can be used with a grayscale texture to
attenuate.

Page 341

Texture projections
.
EnSight provides two mechanisms which may be used to define where a texture should appear on a part. The
first is by projection.
In this mode, it helps to think of the texture as a projected light-source, like a presentation projector, only
without divergence (i.e. the light lines are parallel). The user places the light source to shine through the
scene at some orientation centered at some point. Textures are not limited to the exposed surface in EnSight,
thus any surface that intersects the beam of light is textured
The user can enter the values for this
projection in the "S vector", "T vector"
and "Offset" fields in the dialog.
These define a vector in the space of
the part that will correspond to the
directions of the X and Y axis of the
texture image as well as a point of
focus for the texture.
Perhaps the simplest method for setting
these values is to use the plane tool.
Place the plane tool in the view to
match the desired projection. The
texture will be scaled to fit in the
boundaries of the plane tool with the
texture axis aligned with the tool X and
Y axis. The texture itself is projected
along the Z axis of the tool. Once the
tool has been placed, click on 'Get proj
from plane tool' to fill in the dialog
fields.

The 'Set plane tool to proj' will move
the plane tool to the projection formed
by the current dialog values.

The example below illustrates the placement of a logo, in decal mode with clamp and repeat modes set. Notice
that the texture appears both in front of and behind the tool.

Page 342

The texture projection can also be
specified relative to a point or a collection of
points.
The 'Projection' option menu in 'Absolute'
mode will set the texture projection to the
current settings which places the texture at
an absolute position and attitude in space.
If the part geometry moves or deforms, the
texture remains fixed in the scene, thus it
appears to move on the part surface. The
'Offset relative to ID', allows the user to
specify a node ID in the 'Origin' field.
The 'Offset' X,Y,Z values are considered to
be relative to this node ID. If it moves in
time, the texture projection will appear to be linked to it.
Likewise, 'Offset and S/T vecs relative to node Ids' allows for three
node Ids to be specified, causing the projection to rotate and scale
with the relative positions of those nodes. If one turns on one of
these relative modes, one may need to click 'Get proj from plane
tool' to set up the field values to match the plane tool again (The get
proj option always honors the current relative projection and node
IDs, if provided).
The second form of projection EnSight supports is via 'Variables'.
In this mode, one or two scalar variables are used to provide explicit S and T texture
coordinates for texturing. This is the most general mechanism for texturing. The S-variable
and T-variable option menus provide a list of possible scalar variables.
Users may also set the S and/or T value to the constant quantity 0.5. The variables are
generally in the range [0,1], which map to the edges of the texture map, just inside the border.
Values outside this range will either be mapped to the texture border color (in the case of
clamp mode) or will be warped back into the range of [0,1] by repeated subtraction/addition (in
repeat mode). This form of projection is capable of emulating the previous model. It also
makes it relatively easy to create two dimensional data palettes. Just like the existing palette
in EnSight, some function of a variable is used to select a color from a table. In this case, the
table is a 2D texture, so this can be done for two different variables at the same time, and the
opacity can be varied as a function of those variables.
All forms of EnSight part displays can be textured: surfaces, lines, points, etc. Of special note,
in "variable" mode, points are rendered with a single texture coordinate, regardless of the
form they are displayed as. Thus, a point displayed as a sphere can only use a single pixel
sample from a texture. Thus, to place a logo on a point rendered in sphere mode, one would
need to use 'projection' mode.

Page 343

BASIC OPERATION
How to place a logo on a part
One common use of textures is to place a logo or "decal" onto
a part. This operation involves using a projected texture. This
is a simple three step process.
For this example we will use the AMI dataset which comes
with the EnSight distribution.
1. Load the AMI dataset and set the display type to
shaded surface.
Orient the hypersonic body as shown and select it in the
part list.
2. Next we need to set up the texture map to use.
Select the color icon to bring up the Part Color dialog and
click on the Edit Textures… button to bring up the texture
dialog.
Right click on the first texture button and select 'Load
texture file…'.
Browse to the image file containing your logo image.
A good example is the CEI logo found in CEI_HOME/
ensight92/freedesktop/ensight92.png. This image includes
an alpha channel that is zero outside of the logo pixels (the
'Display Alpha' menu option will display only this channel').
Associate this texture with the part by depressing the icon
that has this image on it.
The hypersonic body will get a tiling of CEI logos over it,
since we only want a single logo, change the Repeat mode
to 'Clamp' (the logos will likely disappear).

3. Finally, we need to set up the transform necessary to
place the logo.
Bring up the plane tool and size/
position it as illustrated:
The key here is to think of the plane
tool as a "flashlight" that shines down
the plane tool's Z axis and the light is
bounded by the plane rectangle.

Once you have the plane positioned, click on 'Get proj from
plane tool'.
The logo texture will now be displayed on the body at the
location specified by the plane tool.

Page 344

ADVANCED USAGE
How to use textures as palettes
EnSight textures can also be used as multi-dimensional
palettes to allow the user to control the color and opacity of
a part based on arbitrary functions of two variables. The key
to this technique is generating the appropriate texture map.
In the following example, we will use a texture map found in
the data directory with the "cube" model.
1. Load the cube model and bring up the variable
calculator.
We will need to create an "S" and a "T" variable that will
be used to access the texture.
2. In the calculator, activate all the variables and create
a new variable named 'S' with the expression
'temperature/50.0' (this puts 'S' roughly in the range
[0,1]).
3. Create a variable 'T' that is the expression
'RMS(velocity)'.
4. Create an xyz clip of the mesh as a 'Z' clip and turn
on shaded display.
5. With the clip_plane part selected, open the texture
dialog. Load the file 'dual_gradient.png', included in
the directory with the cube dataset, into the first slot.
Notice that this texture is an opacity ramp along the X
axis and a color ramp along the Y axis.
6. Set the texture mode to 'Replace' and the repeat
mode to 'Clamp'.
7. Now, set the 'Compute texture coordinates by' option
to 'Variables' and pick 'S' and 'T' as the S and T
variable names.
The display will look like the image shown, depending on
the placement of the clip plane. The coloring is relative to
the Velocity of the field, while the opacity of the plane is
relative to the temperature of the plane. This type of
technique can be used with any two variables; the key is
generating a 2D texture map that is meaningful for
ranges of the two variables in question.

Page 345

How to clip an object with a texture
Textures can also be used to manipulate the transparency of portions of
objects in interesting ways. In this example, a texture image with only an
alpha channel will be used to clip into a part to reveal parts inside of it.
1. Load the cube dataset again.
And as in the textures as palettes example:
2. Load the image files 'circle.png' and 'sphere.png' into two texture
slots.
In both cases:
3. Use the right mouse button menu to set the textures' border
color. Change the border color alpha channel value to 255 and
view only the alpha channel.
Notice that the RGB channels are white, but there
is a dark region in the alpha channel of the
images.

4. Create an isosurface of temperature in the mesh as well as a 'Z'
plane clip.
5. Color the plane clip by velocity.

6. Now, select the isosurface part and much like the logo example,
use the plane tool to project the texture onto the isosurface.
In this case, use the circle texture and modulate texture mode and
set the repeat mode to clamp.
The texture will clip through the isosurface as
a projected circle (from the circle in the
texture) to view parts interior to it. The sphere
texture provides a smoother clip. Experiment
with other textures and repeat modes for
other effects. Remember that each part can
have its own texture, each with a different set
of projection settings for highly expressive
visual options.

Here is an example of a clipping texture applied to
dynamic particle traces. The tracer pulses are not
clipped, but the traces are clipped to a projected
circle texture as in the example.

Page 346

OTHER NOTES
Texture implementation limitations
Texturing in EnSight is done using OpenGL and the multi-texture extension. If your graphics card/driver does not
support this extension, texturing will not be allowed in EnSight and the button used to bring up the Textures dialog will
be removed. OpenGL works best with textures that are powers of two in size and every graphics card has a different
limit on the maximum size of a texture. EnSight will internally scale any input texture (via bilinear interpolation) to fill
the nearest power of two sized rectangle. This can result in much larger textures being used than users might expect
and it can cause interpolated pixels to be used in textures. Also, if textures are too large, EnSight will down-sample
them to the resolution the driver supports. For maximum performance and efficiency, use natural power of two sized
textures where possible and avoid extremely large textures.
A common performance issue users encounter with textures in modulate or replace mode revolves around
transparency. If a texture includes transparent pixels (or transparent border pixels), it is possible that the part could
become transparent. In this case, EnSight is required to sort the polygons of the part to ensure proper occlusion. This
process can be very expensive and slows down rendering significantly. The user can avoid requiring the expensive
sorting, by using textures with solid (or no) alpha channel. If a texture uses only entirely opaque or transparent pixels
and the interpolation option is set to nearest neighbor, EnSight will recognize that it is not possible to have translucent
pixels and will not be required to sort the polygons. This can be used to improve interactive performance and further
enable the use of textures as selective clipping operations in modulate mode.

SEE ALSO
User Manual: Part Operations

Page 347

Animate
Animate Transient Data

INTRODUCTION
Transient data can be animated through EnSight’s flipbook capability. During the flipbook load process, all parts
(both model and created) are automatically rebuilt (if necessary) using the data from each time step in sequence. At
each step, a graphical “page” is created and stored in memory. When the flipbook is active, the pages are displayed
in order as rapidly as the hardware allows (although you can slow it down). You can also step through pages
manually.
The graphical pages can be one of two types: object or image. An object flipbook saves each page as 3D geometry
so you can continue to manipulate the model (e.g. rotate or zoom) during playback. However, for very large models
and/or long sequences, the memory requirements can be substantial. In this case, you can create image flipbooks
that save only the image pixels for each page. Although the size of each page is now fixed, you cannot change the
viewing parameters without reloading the flipbook.
This article covers using the flipbook capability for transient data (and assumes that you have successfully loaded
your transient data). See How To Create a Flipbook Animation for more details on flipbooks. EnSight’s keyframe
animation capability also works with transient data and provides a flexible mechanism for synchronizing your
available time steps with the output animation frames. See How To Create a Keyframe Animation for more
information.

BASIC OPERATION
Prior to loading the flipbook, you should create all parts of interest (e.g. clips, contours, isosurfaces, etc.). These parts
will automatically be recalculated for each time step. To load a transient flipbook:

4. Select the desired page type (Object or
Image).
1. Click the Flipbook Animation icon in
the Feature Icon Bar.
2. Be sure that the Load tab is selected.
3. Be sure the Load Type is set to
Transient.

5. If desired, reset the current beginning and
ending time.
(Clicking this button will replace the
Flipbook Quick Interaction area with the
Solution Time Quick Interaction area.
When you are done, click the Flipbook
animation... button to return).
6. If desired, you can specify a time
increment for the load.

7. Click Load.

For example, using 0.5 would create pages
representing time steps 0, 0.5, 1, 1.5, 2, 2.5,
etc. The in-between steps are calculated by
linear interpolation.

Page 348

The Load Flipbook Status dialog will open and show the progress of the load. You can cancel the load by clicking the
Cancel button and retain all the pages loaded to that point. Once the load is complete, you can run the flipbook using
VCR type controls:
After a flipbook load, the next 3 steps will
generally be the default already.
1. Make sure the Run tab is selected.
2. Make sure the Display is set to
flipbook pages.
3. Click the run forward or backward
button.
The flipbook will begin to run.
OR
You can also step through the pages
manually:
3. Click the forward/backward single
step buttons (once for each page).
You can also enter values in the Current
Page field (and press return) to jump to a
specific page.
4. To change the range of displayed pages, enter new
values in the Begin Page and/or End Page fields (and
press return) or click and drag the left/right slider
handles.
5. To change the display speed, enter a new value in the
Display Speed field (and press return) or simply slide
the slider.
A speed of 1.00 represents “full” hardware speed with no
delays; a value of 0.5 is half of full speed.
6. To cycle the page display, click Cycle.
Cycle will replay the pages in reverse order when the last
page is reached.
7. To stop the animation, click the stop button.
8. When done, set the Display to “original model” instead
of “flipbook pages”.

Record
Once a flipbook is loaded, it can be recorded.
The “Record current graphics window animation”
icon will be on.

Off

On

Click it to open the Save Animation dialog.
This is explained in How To Print/Save an Image

Page 349

Delete
Any type of flipbook can be deleted:
1. Click Delete... in the Flipbook Quick Interaction Editor.
2. Confirm the deletion.
All memory associated with the flipbook is freed.

ADVANCED USAGE
If you have created transient particle traces (pathlines) and set up a particle trace animation, you can also load a
flipbook and show the particle trace animation synchronized with the flipbook. The trace animation will automatically
play through the time range of the flipbook and stay in sync with the flipbook pages. See How To Create Particle
Traces and How To Animate Particle Traces for more information.

OTHER NOTES
Since both object and image flipbooks build pages from the current set of parts based on their current attributes, if
you make a change (such as color a part by a different variable or create a new part), you must reload the flipbook.
There are exceptions. With an object flipbook, you can make a part invisible while the flipbook is running.

SEE ALSO
How To Load Transient Data
How To Print/Save an Image
How To Create a Flipbook Animation
User Manual: Flipbook Animation, Flipbook Animation

Page 350

Create a Flipbook Animation

INTRODUCTION
Various types of data can be animated through EnSight’s flipbook capability. During the flipbook load process,
selected parts are automatically rebuilt based on some criteria (such as a delta for a clipping plane). For each step, a
graphical “page” is created and stored in memory. When the flipbook is active, the pages are displayed in order as
rapidly as the hardware allows (although you can slow it down). You can also step through pages manually.
The graphical pages can be one of two types: object or image. An object flipbook saves each page as 3D geometry
so you can continue to manipulate the model (e.g. rotate or zoom) during playback. However, for very large models
and/or long sequences, the memory requirements can be substantial. In this case, you can create image flipbooks
that save only the image pixels for each page. Although the size of each page is now fixed, you cannot change the
viewing parameters without reloading the flipbook.
There are four distinct types of flipbooks:
Transient

Pages are constructed by stepping from the current beginning to ending
time range and rebuilding all time-dependent parts based on each time
step in sequence.

Mode Shapes

Pages are constructed by applying a cosine-driven scaling factor to a
displacement variable.

Create Data

Pages are constructed by applying a delta to either a clip part or an
isosurface.

Linear Load

Pages are constructed by applying linear interpolation ranging from zero
to the maximum (displacement) vector field value.

This article covers only the “Create Data” type of flipbook. See How To Animate Transient Data for details on
transient flipbooks. See How To Display Displacements for details on mode shape flipbooks.
For more sophisticated animations, use EnSight’s keyframe animation capability.

BASIC OPERATION
For each page of the flipbook, a delta value will be applied to all active clip parts and isosurfaces. For clips, the delta
represents a translation vector; for isosurfaces it is an increment to the isovalue. There are two ways to specify these
delta values: either through interactive manipulation or via the applicable Feature Detail Editor for the part. The
former method is discussed below, the latter in the Other Notes section at the end.
Prior to loading the flipbook, you should create all parts that you wish to animate (clips and/or isosurfaces) and

Page 351

manipulate the part so that it is in the desired location for the start of the flipbook. To load the flipbook:

4. Select the desired page type (Object or
Image).
1. Click the Flipbook Animation icon in
the Feature Icon Bar.
2. Be sure that the Load tab is selected.
3. Be sure the Load Type is set to
Create data.

5. Set the desired number of pages.
The delta value will be added to the appropriate
entities for each page
6. Click Start to begin recording interactive
part manipulations.

6a. For clipping plane parts, reopen the Quick Interaction area for the part
(double-click on the part in the Main Parts list).
6b. Toggle on Interactive Tool, move the mouse into the Graphics Window and
interactively position the tool to the desired location for the end of the
flipbook.

6a. For isosurface parts, reopen the Quick Interaction area for the part (doubleclick on the part in the Main Parts list).
6b. Change the Interactive Pulldown to Manual and adjust the slider until the
isovalue is as desired for the end of the flipbook.
7. Return to the Flipbook Quick Interaction area (i.e. perform step 1 again).
8. Click Stop to end recording interactive Iso/Clip.
9. Click Load.
10. Save playing animation to file (must be playing to save)

Page 352

The Load Flipbook Status dialog will open and show the progress of the load. You can cancel the load by clicking the
Cancel button and retain all the pages loaded to that point. Once the load is complete, you can run the flipbook using
VCR type controls:
After a flipbook load, the next 3 steps will
generally be the default already.
1. Make sure the Run tab is selected.
2. Make sure the Display is set to
flipbook pages.
3. Click the run forward or backward
button.
The flipbook will begin to run.
OR
You can also step through the pages
manually:
3. Click the forward/backward single
step buttons (once for each page).
You can also enter values in the Current
Page field (and press return) to jump to a
specific page.
4. To change the range of displayed pages, enter new
values in the Begin Page and/or End Page fields (and
press return) or move the slider range markers.
5. To change the display speed, enter a new value in the
Display Speed field (and press return) or simply slide
the slider.
A speed of 1.00 represents “full” hardware speed with no
delays; a value of 0.5 is half of full speed.
6. To cycle the page display, click Cycle.
Cycle will replay the pages in reverse order when the last
page is reached.
7. To stop the animation, click the stop button.
8. When done, set the Display to “original model” instead
of “flipbook pages”.

Record
Once a flipbook is loaded, it can be recorded.
The “Record current graphics window animation”
icon will be on.

Off

On

Click it to open the Save Animation dialog.
This is explained in How To Print/Save an Image

Page 353

Delete
Any type of flipbook can be deleted:
1. Click Delete... in the Flipbook Quick Interaction Editor.
2. Confirm the deletion.
All memory associated with the flipbook is freed.

OTHER NOTES
Rather than specify the part delta values through interactive part manipulation as described above, you can set the
values explicitly using the Feature Detail Editor for the part. For clip parts:
1. Select Edit > Part Feature Detail Editors > Clips... to open Feature Detail Editor (Clips).
2. Select the desired part in the parts list of the Feature Detail Editor (Clips).
3. In the Animation Delta section, enter the desired values in the X, Y, and Z fields and press return.
For isosurfaces:
1. Select Edit > Part Feature Detail Editors > Isosurfaces... to open Feature Detail Editor (Isosurfaces).
2. Select the desired part in the parts list of the Feature Detail Editor (Isosurfaces).
3. In the Animation Delta field, enter the desired isovalue delta value and press return.
When a flipbook is subsequently loaded, active clips and/or isosurfaces will update based on these animation delta
values.

Since both object and image flipbooks build pages from the current set of parts based on their current attributes, if
you make a change (such as color a part by a different variable or create a new part), you must reload the flipbook.
There are exceptions. With an object flipbook, you can make a part invisible while the flipbook is running.
NOTE:
Alpha transparency does not work correctly during flipbook animation because sorting is not done. The final image
will generally show this lack of proper sorting. To view transparency during animations, use the solution time
streaming or keyframe animation.

SEE ALSO
User Manual: Flipbook Animation

Page 354

Create a Keyframe Animation

INTRODUCTION
EnSight’s ability to handle large, transient datasets has led to its use in the production of many video animations of
engineering and scientific data. EnSight uses a keyframe animation system. A keyframe is a set of viewing
parameters that specify a particular view of the scene in the Graphics Window. The view may be notable because of
what is visible, or because the view represents the transition point from one scene to another. Once a set of
keyframes has been selected, EnSight can automatically generate frames to interpolate the viewing parameters
between keyframes for a smooth animation.
The changes to viewing parameters between keyframes are not limited to simple rotations, translations, or zoom
operations. You can also use EnSight’s frames capability to move parts independently, e.g. to animate an exploded
view of a complex assembly. You can also animate the global look-from and look-at points for “fly-by” style
animations.
While refining your animation, you can display it directly in the Graphics Window. When complete, you can specify
the output resolution (e.g. for NTSC or PAL video) and set the recording device (e.g. to a disk file).
Although the production of adequate animation is easy, good animation takes experience. A sequence that looks
good on your high resolution workstation screen may look less than acceptable when transferred to VHS videotape.
An object rotating in ten degree increments may be an appropriate speed for your workstation graphics. At thirty
frames per second, however, the rotation will complete in just over a second – too fast for normal viewing. See the
Other Notes section for some additional hints and tips.

BASIC OPERATION
All keyframe animation functions are controlled through the Keyframe Quick Interaction area. You can define the
transformations between keyframes, or you can create standard animations

To define your own keyframes:
1. Click the Keyframe Animation icon in the Feature Icon bar.
2. Set all viewing parameters to the desired location for keyframe 1.
3. Click Create Keyframe to save the first keyframe.
Note that the Keyframing toggle is automatically switched on
when you begin saving keyframes.
4. Change the viewing parameters to the desired location
for keyframe 2.
5. Click Create Keyframe to save keyframe 2.
You can play your animation at any time to check your results.
The animation will play the keyframe range specified in the
Run From/To fields in Run Attributes...
6. Click Run Animation to play the animation.

Important Notes!
You can abort a running animation by
moving the mouse into the animation
display window and pressing the ‘a’ key.
If you toggle-off the Keyframing button, any
keyframes currently defined will be deleted.
If you wish to save a set of keyframes, click
the Save... button.

7. Continue to change viewing parameters and click
Create Keyframe until you have saved all desired
keyframes.

Page 355

There are many ways to specify the desired transformations between keyframes. See the following articles for more
information:
How To Rotate, Zoom, Translate, Scale
How To Create and Manipulate Frames
How To Set LookFrom/LookAt
How To Define and Change Viewports

To Create Keyframes using Predefined Animations:
1. Click the Keyframe Animation icon in the Feature Icon bar.
2. Set all viewing parameters to the desired location for keyframe 1.
3. Click Quick Animations... to bring up the Keyframe Quick Animations Dialog.
In this dialog you will be able to create keyframes which define transformations which will (a) fly the viewer
around your model, (b) rotate your model, or (c) create exploded views of your parts. Any one of these, or a
combination may be used.
4. Set the number of frames which will be
created
5. Acceleration at the first and last
keyframes that will be created is on by
default. If you do not want to accelerate/
decelerate toggle these off.
6. Toggle Fly Around on if you wish to move
the viewer (camera) in a circle.
(a) You can choose Right (start the viewer
moving to the right) or Left.
(b) Specify the number of revolutions.
7. Toggle Rotate Objects if you wish to rotate
the scene.
You can rotate positively or negatively about
all three axis. For each axis you set the
number of revolutions.
8. Toggle Explode View if you want your
parts to be translated in reference to an
origin.
You can specify the origin or set the origin to
the transformation center.
Direction sets the explode direction and can
be one of:
X,Y,Z - translate in the coordinate direction
XYZ - translate in the dominant coordinate direction
Radial - translate in the direction from the origin
specified through the part centroid

The part that is farthest from the origin
specified will be transformed Distance units

9. Click Create Keyframes to create the
keyframes which will transform according
to the selections made.

Page 356

The following sections provide details on the animation control dialogs opened from Run Attributes... in the
Keyframing Quick Interaction area.
Speed/Actions
The Speed/Actions tab allows you to set the number of sub-frames between each pair of consecutive keyframes as
well as specify run attributes such as acceleration and commands to execute:
1. Click Run Attributes... in the
Keyframing Quick Interaction area
to bring up the Keyframe Run
Attributes dialog.
2. Click the Set Speed/Actions tab.
3. Select the desired keyframe to
edit: either enter the value or use
the up/down buttons.
4. Enter the desired number of subframes between the keyframe
selected in step 1 and the next
(the default is 20).
5. If desired, set the number of
frames to hold for the keyframe
(default is 1).
6. If desired, enter EnSight
commands to execute when the
selected keyframe is reached. The
command(s) will be executed
before the frame is displayed.
7. If you added or changed the
commands to be executed at a
keyframe, click Update
Commands.

8. If you want the transformation to accelerate out
(or into) the keyframe, toggle Acceleration on.
9. Continue by selecting a new keyframe to edit
and click Close when done.

Use Interactive Iso/Clip
By turning this toggle on, any clip or isosurface interactively moved
during the keyframe will animate.
Animate Transparency Change
By turning this toggle on, transparency changes to parts during the
definition of the keyframes will be part of the animation.
The number of sub-frames controls the speed with which objects transform between keyframes. More sub-frames
yields slower motion.
You can insert any valid EnSight command to be executed at a keyframe. If your command sequence is more than a
few lines, it is best to save the sequence in a file and just enter the command play: filename. There is a special
case of executing a command at a keyframe. If you insert the command shell: filename, The file filename
(which is assumed to be a UNIX executable command) will be executed after each sub-frame and each surrounding
keyframe. In addition, if you are saving animation frames to disk files, the name of the image file just written is
passed to the executable as the first argument. This capability can be used to postprocess the image files, for
example to resize and re-sample an image or copy it to a different location. If this capability is used, the shell:
filename command must be the only command specified.

Page 357

Viewing Window
The Keyframe Viewing Window tab allows you to set the size and location of the animation display window:
1. Click Run Attributes... in the Keyframing
Quick Interaction area to bring up the
Keyframe Run Attributes dialog.
2. Click the Viewing Window tab.

3. Select the desired window type:
Normal Use the current Graphics Window
(initially 794 x 659)
Full

4. Click Close.

Use the full screen with no window
borders (typically 1280 x1024)

NTSC Use NTSC video resolution (640 x 480)
and position at the lower-left corner
PAL Use PAL video resolution (720 x 576)
and position at the lower-left corner
User Defined
Detached Display

Use the Min/Max X and Y settings
Use the detached display and set Min/
Max settings

The Min setting for User Defined specifies the position of
the lower-left corner of the animation window (as an offset
from the lower-left corner of your monitor screen). The Max
setting is the upper right corner of the animation window.

Page 358

Run From/To
The Run From/To tab allows you to specify the range of keyframes to play.
1. Click Run Attributes... in the
Keyframing Quick Interaction area to
bring up the Keyframe Run Attributes
dialog.
2. Click the Run From/To tab.
3. If you wish to limit the animation
playback to certain keyframes set the
Run From and To fields. By default they
are set to cover all of the keyframes you
have created.

Page 359

Transient
If you have transient data you can specify how it will be used during the keyframe animation.
1. Click Run Attributes... in the
Keyframing Quick Interaction area to
bring up the Keyframe Run Attributes
dialog.
2. Click the Transient tab.
3. Toggle Use Transient Data on if you
want to use transient data during the
animation.
Transient data does NOT have to be on
(and should not) to play back a flipbook
animation during the keyframe animation.
4. Timelines allow you to use transient
data during each defined timeline.
If the timelines do not cover all of the
keyframes you will have a portion of your
animation with no transient data.
By default a single timeline exists which
covers all of the defined keyframes. To
create more timelines click New
5. For each timeline you can specify the begin and
ending time value (either step or simulation time See Solution Time dialog).
6. Time will be interpolated such that the Start Time
occurs at the Start At Keyframe and the End Time
will occur at the End At Keyframe unless the Specify
Time Increment is toggled on. If the Specify Time
Increment is on each frame during the timeline is
incremented by the time indicated.
If the Start Time or End Time is encountered before the
Start At or End At Keyframes the transient data will either
Loop (go back to the Start Time) or Swing (play in
reverse).
Record...
The Keyframe Animation Recorder dialog specifies the type of recording device:
1. Click Record... in the Keyframing Quick
Interaction area.
2. Toggle on Record To File.
3. Select the desired file format and
options.(see below).
4. Provide the File prefix.
5. Set other Advanced options.
The file format, prefix, and other options
are described in How To Print/Save an
Image
6. Click Close.

Page 360

Save and Restore
A set of keyframes and related information can be saved to disk and later restored. To save keyframes:
1. Click Save... in the Keyframing Quick Interaction area.
2. Enter the desired file name in the File Selection dialog and click Okay.
To restore previously saved keyframes:
1. Click Restore... in the Keyframing Quick Interaction area.
2. Enter the desired file name in the File Selection dialog and click Okay.

OTHER NOTES
As pointed out in the introduction to this article, high-quality animation takes time and experience. CEI has produced
a great deal of animation over the years and has learned a variety of lessons. In the hope that EnSight users can
avoid many of the pitfalls inherent in the process, many of these lessons and rules of thumb are presented here.
EnSight’s keyframe animation methodology is borrowed from the animated film industry. In making animated films,
the master animator defines how the scene will look at certain points in time (the keyframes) and then hands the work
off to an “in-betweener”, with instructions on how many frames to add between each pair of keyframes. The inbetweener then draws the missing frames. EnSight’s approach is similar with the user as the master animator and
EnSight as the in-betweener. Some of the strengths of this approach include:
1. When keyframing is on, EnSight is not only recording the viewing parameters when you click Create Keyframe, it
also records the actions taken to get from the last keyframe to the current one. This approach permits certain
operations to be performed without ambiguity (such as rotating by 180 degrees or more).
2. Each Viewport can be animated independently.
3. Flipbooks can be played during an animation.
4. Animated particle traces can be played during an animation.
5. Transient data is easily synchronized with the generated frames. When the animation is run, EnSight will
automatically step through time and recalculate all time-dependent entities.
6. Output can go directly to disk files for later recording, manipulation, or conversion to other formats (e.g. MPEG or
QuickTime).
7. Additional power and flexibility can be achieved since EnSight command language statements can be issued at
keyframes.
The keyframe capability was designed to enable engineers and scientists to produce quality animation. As such, it
lacks most of the more elaborate controls available in commercial animation packages (which typically cost 2-3 times
more than EnSight). Some limitations:
1. Only transformation parameters (global, frame and camera transforms) are saved through the keyframing
process. Other parameters and part attributes are not interpolated between keyframes.
2. Light sources are fixed in EnSight – they cannot move during the animation.
3. The shading and lighting model used by EnSight is fairly simplistic.

Tips for Video Recording
Animation Holds
Whenever an animation is started or stopped use a “hold” to allow your viewers to establish the visual context of the
scene. A hold of 3 seconds at the beginning and 2 seconds at the end usually works well. For complex imagery,
longer holds may be required. Note that a hold can typically be performed at the recording level – it is not necessary
to have EnSight compute multiple frames for a hold.
Rate Control
The speed at which events occur during an animation is one of the most difficult aspects to master. Viewers become
Page 361

confused and disoriented if motion is too fast; too slow and your viewer may lose interest. The frame rate for NTSC
(the video format used in North America) is 30 frames per second. Although there is a great deal of variation
(depending on graphics hardware speed and model size), your workstation will typically have a much slower frame
rate. Therefore, what appears to be good speed on your workstation may be much too fast when recorded to video
at 30 frames per second.
Trial and error is one method to determine proper rates. Although you may end up doing some “line test” video
recording to refine your rates, use the method described here to derive good starting values:
1. Define all the keyframes.
2. Set up the animation to play back at full screen.
3. Set up the animation to play only from the first to the second keyframe.
4. Set the number of sub-frames between keyframes 1 and 2 to be 300.
5. Select View > Bounding Box > Static Box.
6. Using a watch with a second hand, time how long it takes to play the animation. Call this time “T”. We know that
it will take 10 seconds to play 300 frames on video. Compute the following:
factor = T/10.
For example, if you find T to be about 12 seconds, then factor is 1.2, which means that the rate you see on the screen
is 1.2 times slower than what you will see on video.
7. Iteratively adjust the number of sub-frames between keyframe 1 and 2 (running the animation after each
adjustment) until you like the rate you see on the screen.
8. Finally, adjust the number of sub-frames by the factor found in step 6. For example, if 150 sub-frames were
required for a good rate of speed, then change the number of sub-frames to 150*factor to see the same rate on
video.
9. Perform steps 3 through 8 for the next set of keyframes.
Transient Data
Animation is particular useful for presenting transient data. However, since both viewing parameters and time can
change simultaneously, the potential for confusing viewers is very high. In general, you should never change both
viewing parameters and time simultaneously. It is typically much better to use transformations in an opening scene to
present the model to the viewer. The transformations should end at a vantage point suitable for viewing the transient
phenomena. At that point, the time-dependent data can be displayed. If you must alter the scene during transient
display, do so with great care to avoid disorienting viewers.
Note that you can animate time-dependent information without transformations by merely creating two keyframes
without performing any transformations between them.
In many instances, there will not be enough time steps in the simulation to produce an animation of adequate
duration. If the simulation does not involve changing geometries, EnSight can interpolate between time steps
(linearly) to yield additional frames. However, keep in mind that your simulated phenomena is almost certainly not
linear in nature. If you have EnSight generate more than a few interpolating frames between each actual time step,
the resulting discontinuity at keyframes (from the piece-wise linear interpolation) is quite visible in the resulting video.
Frame count
The total number of frames that EnSight will produce during the animation is the sum of all sub-frames plus the
number of keyframes. This is especially important to keep in mind when synchronizing transient data with animation
frames.
Animated Traces
If you display animating particle traces during keyframe animation, you may have noticed that the trace animation
always resets at the beginning of the keyframe animation. However, in most cases it is desirable to have the trace
animation fully in progress when the animation begins. This can be accomplished by creating an additional keyframe
at the beginning of the animation. Set the number of sub-frames between keyframes 1 and 2 to a value high enough
to yield the desired tracer saturation. When you run the animation, set the Run From field to 2 so that the animation
begins generating frames with keyframe 2. At that point, the tracer animation process will have executed once for
each sub-frame between keyframes 1 and 2.
Page 362

Color
The color gamut (the range of colors a device is capable of displaying) of video (especially NTSC) is significantly less
than that of your workstation monitor. The result is that certain colors that look fine on your workstation cannot be
reproduced on video. Fully saturated colors (especially red and blue which “bleed” across the screen) are particularly
troublesome. However, it is quite easy to de-saturate your images prior to recording. There are actually three ways
to do this:
1. Modify all of the colors in use to de-saturate them. For example, if a color is pure red (1., 0., 0.), change it to be a
more pastel red (.85, .1, .1).
2. Modify the saturation factor in the Image Format Options. A factor of 0.85 is usually good.
3. Create your animation, then de-saturate the images using an image tool such as the one available from the San
Diego Supercomputing Center (it’s free). This will only work, of course, if you are saving animation images to disk
files.
Dark backgrounds work much better than light backgrounds. Black is often the best choice.
Lines
Moving single-width lines have a tendency to “crawl” on video. Use a minimum line width of 2.
Anti-aliasing
Without correction, computer-generated imagery exhibits aliasing artifacts that typically show up as jagged edges.
For our purposes it is sufficient to say that aliasing results from sampling at a resolution too low to capture the “signal”
represented by the underlying geometry. We can only sample our geometry at the available pixels. Since the
effective number of pixels in the NTSC video signal is only one quarter the number of your workstation screen, what
looks fine on your workstation may be less than acceptable on video. EnSight provides direct anti-aliasing support
through its multipass capability. There are also some other ways to mitigate this problem.
1. If you are recording images from EnSight directly to a video recorder, use a scan converter (a piece of hardware)
to filter full screen images to NTSC resolution images.
2. If you are recording images to disk files, record them at full screen resolution and then use an image re-scaling
tool (such as izoom on SGI hardware) to down-sample the images to the desired video resolution. This downsampling averages several pixels to yield one output pixel, effectively preserving much of the resolution contained
in the original full screen image.
Annotation
The smallest annotation text that can be clearly read on video has a font size of 40. For title sequences, use a size of
about 65.
If you display parts colored by variables, you should always include the applicable color legend so viewers
understand what the coloration represents. For color legends, it is often sufficient to display just one value at the top
(the maximum) and one at the bottom (the minimum) in addition to the name of the variable. In fact, sometimes just
using “High” and “Low” are sufficient if only the relative magnitudes of the variable are important.
Screen Space
The region of a video display that is “safe” for viewing is typically smaller than your animation display window. You
should plan your scenes such that objects of interest (especially annotation entities) do not come “too close” to the
edge. If you keep these objects within the range (in EnSight viewport coordinates) .06 to .94 for X (width) and .05 to
.95 for Y (height) you should be safe.
Introductory Sequence
Your animation should begin with some title slides explaining the problem domain to your viewers. Try not to put too
many words on any one slide and display each one for at least four seconds.
Next, before displaying your results, provide a sequence that introduces viewers to your model. This sequence
should be long enough and complete enough to orient the average target viewer to your problem. It is difficult to
overestimate the need for this sequence. Without it, viewers are often confused and disoriented for the entire
animation.

Page 363

Credits
You should always include proper credits on any animation you produce. Even animations initially intended only for
internal consumption often end up shown to broader audiences.
Stretching an Animation
Ten minutes of video requires 18,000 frames. Only after you have created your first animation will you realize that this
can represent a logistical nightmare. In many cases, you can reduce the number of generated frames required using
each frame multiple times. If you record two video frames for each actual frame you have, in effect, slowed your
animation by half since there are only 15 new frames per second. Although 15 frames per second produces less
smooth motion than 30, it is still usually acceptable. Further reduction however, say to 10 unique frames per second,
produces noticeable jerkiness.

The Recording Process
There are three basic ways to go about recording your animation:
1. The cheapest method (and the one that typically yields the poorest results) is to simply record the animation
directly off the workstation. This can be done either by pointing a video camera at the screen or using the built-in
video out signal available on some workstations.
Although this may be suitable for some simple steady-state problems, the resulting video is usually of very poor
quality. Note also that the frame refresh rate is dependent on the complexity of your geometry (which can vary
throughout the animation) and the speed of your hardware.
2. EnSight can also write each generated frame to a disk file. Given the current state-of-the-art in hardware and
software for video production, this is the preferred method. The images can be further manipulated on disk (e.g.
color de-saturation or pixel averaging) prior to recording. If a problem occurred, missing or bad frames can be
regenerated. Tools also exist to convert sequences of image files to popular animation formats such as MPEG and
QuickTime.
3. EnSight can directly output popular animation formats, including MPEG, AVI and its own format - EnVideo.

SEE ALSO
User Manual: Keyframe Animation

Page 364

Animate Particle Traces

INTRODUCTION
EnSight’s powerful particle tracing facility can trace particles (either steady-state or transient) through flow fields.
Animating the resulting traces often promotes intuitive comprehension of the characteristics of the underlying flow
field. Traces are animated by displaying one or more tracers on all traces of the trace part. A tracer moves along the
path of a trace with length proportional to the local velocity. EnSight provides complete control over all aspects of the
tracers including length, speed, and release interval for multiple pulses.
This article covers particle trace animation and assumes that you have already created one or more particle trace
parts. See How To Create Particle Traces for more information.

BASIC OPERATION
To enable particle trace animation and adjust the animation parameters:

1. Double-click the desired particle trace part in the Main Parts list.
2. Toggle on Animate in the Quick Interaction area.
3. Click Animate to open the Trace Animation Settings dialog. Make changes as desired (remember
to press return for changes to text fields).
Set the color of the tracers to either Trace
Color (i.e. the same color as the parent
trace part) or Constant (and set the desired
color using the Mix... button or the RGB
fields.
Set the line width of the tracers.
If transient traces (pathlines), set the Start
Time and/or Max Time.

Set the tracers length factor (see below).
Set the tracers speed factor (see below).
Set tracers head representation. Either
None or Spheres. If Spheres, the radius can
be Constant (set by the Scale value) or
sized by a variable and scaled by the Scale
value. Sphere detail set via Detail field.

Click to load good default values to the
Tracer Time, Tracer Delta, and Pulse
Intervals fields.

Toggle on Multiple pulses and set the
interval between pulses (see below).

Page 365

Tracer Parameter Descriptions:
Tracer Time (Length)

The Tracer Time (Length) parameter acts as a scaling factor for all tracer lengths
(the higher the value the longer the tracer). Tracer length varies as the local
velocity changes along the trace. For example, the tracer will lengthen as the
leading edge of the tracer moves into a higher velocity region.

Tracer Delta (Speed)

The Tracer Delta (Speed) parameter acts as a scaling factor for the tracer speed
(the higher the value the faster the tracer). The speed of the leading and trailing
tracer edges varies as the local velocity changes along the trace.

Pulse Interval

The interval between successive tracer emissions when in multiple pulse mode
(the higher the value the longer the interval between pulses). Note that the
distance between tracers will increase when the local velocity increases.

Record
Once animated traces are computed,they can be recorded.
The “Record current graphics window animation”
icon will be on.

Off

On

Click it to open the Save Animation dialog.
This is explained in How To Print/Save an Image

ADVANCED USAGE
If you have time-dependent data and have calculated transient particle traces (pathlines), you can enable trace
animation, load a transient flipbook, and view the animating pathlines simultaneously with the dynamic flipbook. See
How To Create Particle Traces and How To Animate Transient Data for more information.

OTHER NOTES
The parameters in the Trace Animation Settings dialog are not specific to the currently selected particle trace part –
the settings apply to all currently animating particle trace parts.

SEE ALSO
User Manual: Particle Trace Animation

Page 366

Annotate
Create Text Annotation

INTRODUCTION
EnSight has comprehensive features for text annotation. Not only can you display and position user-specified text,
you can also display text contained in the description lines of some data formats as well as dynamic text that changes
over time.

BASIC OPERATION
1. Click Annot in the Mode Selection
Area.
2. Click Text icon from the Mode Icon Bar
to open the Annotation dialog.
3. Click the New button, which will open
the Text annotation editing dialog.

4. Enter the desired text, and hit the Update
text button.
The text should now show up in the graphics
window.
- OR 4. Click Dynamic update on,
then enter the desired text
and see the text appear dynamically in the
graphics window as you type.
While entering text, you can easily change the
script to super, sub, or normal by clicking the
Superscript, Subscript, or Normal buttons which
will insert , , or  into the string.
Store and Recall buttons allow the user to insert
the  and  codes into the text string
for saving and recalling a text position on the
screen.
Other Special Coded Items, including changing
the font, which can be inserted into a string (by
selecting and hitting Insert special item) are
discussed below.

Page 367

To manipulate text string attributes, first select the string(s) of interest in the list (or while in Annot mode,
pick them in the graphics window), then:
To change visibility:
Toggle Visible off or on. Note that in Annot Mode, the text
will not be completely invisible but will be displayed in a
subdued color.
To change color:
Select the desired color from the matrix, enter RGB
values in the fields, or click More... to open the Color
Selector dialog.
To change justification:
Select the desired Left, Right, or Center justification from
the Justify pulldown.
To change text size:
Either resize the text interactively by grabbing the Resize
Point of the text string (bottom right) and dragging, or by
precisely specifying the font size in the Size field of the
dialog (or using the slider to change the font size).
Important Note! The text size specified is relative to the
size of the Graphics Window. If you increase the size of
the Graphics Window, all text will also rescale to
maintain the same relative size.
To change text rotation:
The orientation of text about the text justification point
may be specified interactively by grabbing the Rotation
Point of the text string (cross shape at upper right) and
rotating the text to the desired orientation, or by precisely
specifying the rotation angle (in degrees) in the Rotation
field (or using the slider to change rotation angle).
To add shadow text effect:
Enter offset and intensity or use sliders
To change location of the justification point in the
graphics window:
Either interactively drag the text to the desired location,
or precisely specify the location in the Origin XY fields.
You can also specify the viewport that the text is to be
positioned relative to. If 0, the position is relative to the
graphics window.

Page 368

Special Coded Items
EnSight can automatically build text strings based on information from various sources. To use one of these special
strings, select the desired item from the Special String list, select any required options, and click Insert Special String.
A code will be inserted into the Text field. If not in Dynamic update mode, hit the Update text button to create the text
entity and display it.
The following special strings are available. If multiple cases are loaded, any reference to parts or variables applies to
the currently selected case (select Case > casename to changes cases)
Fonts

Brings up the TrueType font selection dialog, allowing a new font to be selected
Information on manipulating fonts, including
additional text font formatting codes that can
be used, are described in How To
Manipulate Fonts

Symbols

Brings up a symbol dialog. Click on any symbol to insert it at the current character
insertion point of the string. The symbol will be inserted in to the string via a xxx,
where xxx is the ASCII number for the selected symbol.

Constant Variable

The value of a constant variable (such as Time or Length). Select the variable from the
Constant Variables list and select the desired numeric display format from the Number
Format list.
If the constant variable changes, the corresponding text will automatically update. This
is very useful for displaying the current solution time during a transient animation.

Date

Current date. Example: Wed Jan

Geometry Header

The first or second text line of the geometry file of the current case. Select Line 1 or Line
2.

Measured Header

The first line of the measured (discrete) data file of the current case.

Variable Header

The first line (typically the description line) from a variable file. Select the desired
variable from the Variable(s) list.

Part Value

The “value” of a part. Currently works for isosurface and some (ijk, xyz, rtz, plane
aligned with axis, or attached to spline) clip parts where the value is the corresponding
isovalue or clip location or value. Parts that have a value will appear in the part selection
list. Select the part in the Part(s) list and select the desired numeric display format from
the Number Format list.

Part Description

The description of the part as displayed in the Main Parts list. (Note that you can change
this text by editing the Desc field in the applicable Feature Detail Editor for the part.)

Version

The name and current version number. Example: EnSight Version 6.0.

1 12:34:56 1997

EnSight command language variables can also be inserted into annotation strings via a special item coding option.
This coding item does not have an associated GUI, but can be typed directly into the annotation text edit field. The
coding has the form:
<\\ensv “format“ var_name\\>
The format string is the “C” printf specfication for the item formatting. var_name is the actual name of the variable
value to be inserted. If the following lines of EnSight command language were executed:
$globalstring example
$example = Hello from EnSight
The annotation string:
The value is: <\\ensv “%s“ example\\>

Page 369

would result in the annotation containing the string “The value is: Hello from EnSight”. If the variable is updated, the
following command language will update the annotation:
text: update
Another example uses the built-in EnSight frames per second counter which stores the current rendering rate in
frames per second in the ensight variable “ensight_fps”. This annotation string, containing embedded ensight
variable formatting, will display the current rendering rate dynamically in EnSight:
Frames per second: <\\ensv “%.2f“ ensight_fps\\>
It is also possible to embed the value of an interactive query into an annotation string. The first value of the
interactive query results is always used. The format for this is the keyword "iqval", followed by a format statement
and a interactive query id number (zero based). For example:
Temperature = <\\iqval "%.2f" 0\\>
will display an annotation string with the value of interactive query 0 displayed to two places of precision after the
equal sign in the annotation.

Delete Annotations
Existing annotations can be deleted in the Annotation dialog
or can be selected and the Delete icon can be clicked:

Select All
You can select all of the current annotation type by clicking:

SEE ALSO
How To Manipulate Fonts
User Manual: Annot Mode

Page 370

Create Lines

INTRODUCTION
EnSight can display annotation lines that can either be specified in 2D screen space or in 3D world space.

BASIC OPERATION
1. Click Annot in the
Mode Selection Area.
2. Click Line icon from the Mode
Icon Bar to bring up the
Annotation dialog.

3. Create a new line in the Graphics
Window by clicking the New button.

To manipulate a line attributes, first
select the line(s) of interest in the list
(or while in Annot Mode, pick them
in the graphics window), then:
To change visibility:
Toggle Visible on or off. Note that in
Annot Mode invisible lines are drawn in
a subdued color.
To change color:
Select the desired color from the
matrix, enter RGB values in the fields,
or click More... to open the Color
Selector dialog
To change location:
Set the ‘Origin by’ to Screen
coordinates or 3D coordinates. You
can drag the endpoints specified by
screen coordinates in the graphics
window. But you must drag the 3D
coordinate end points in Part Mode.
You can also specify the X, Y (and Z if
3D coordinates) by typing into the
fields.
To change line width:
Click the Width Pulldown and select the
desired line width.
To label the line:
Specify Text Annotation from the
pulldown to align it with line annotation.
To change Arrowhead status:
Click the Arrows Pulldown and select
the desired state.
To delete a line, click Delete button.

Page 371

SEE ALSO
User Manual: Annot Mode

Page 372

Create 2D Shapes

INTRODUCTION
EnSight can display 2D shapes (arrow, rectangle, and circle in present release). These 2D shapes overlay the
Graphics window and are not associated with any viewport.

BASIC OPERATION
1. Click Annot in the
Mode Selection Area.
2. Click 2D Shape icon from the
Mode Icon Bar to bring up the
Annotation dialog.
3. Create a new shape in the
Graphics Window by setting
the Shape type and then
clicking the New button.

To manipulate a shape’s attributes, first select
the shape(s) of interest in the list (or while in
Annot Mode, pick them in the graphics
window), then:
To change visibility:
Toggle Visible on or off. Note that in Annot Mode
invisible shapes are drawn in a subdued color.
To change color:
Select the desired color from the matrix, enter
RGB values in the fields, or click More... to open
the Color Selector dialog.
To change location:
Either select the shape and drag it to the desired
location, or type appropriate coordinates into the
Origin X/Y fields. The origin of a 2D arrow is the
point of the arrow. The origin of a rectangle or
circle is the center of the object.
To change size:
Either select the shape by the resize handle and
drag it to the desired size, or type appropriate
Width/Length (or Height or Diameter) values into
the fields. Units are 0 to 1.
To change fill mode:
You can draw the shape in filled mode or in outline
mode.

To Apply textures to the shape:
These are the same textures used by the
parts and the ‘Edit textures...’ button will
open the part texture dialog, where textures
or animations can be loaded and other
attributes set. Note that 2D shape textures
always replace the current shape color and
modes like “modulate” and “decal” as well as
custom projections and repeat behavior are not
supported.

Other attributes:To Rotate the shape:
According to the selected shape, other
attributes may exist, such as rotation
attributes, arrowhead attributes, etc.
To delete a shape, click the Delete button.

Page 373

SEE ALSO
User Manual: Annot Mode

Page 374

Create 3D Arrows

INTRODUCTION
EnSight can display 3D arrows. The 3D arrow is defined in model space and transforms with the scene. The 3D arrow
is visible in the viewport(s) specified.

BASIC OPERATION
1. Click Annot in the
Mode Selection Area.
2. Click 3D Annotation Arrow
icon from the Mode Icon Bar
to bring up the 3D Annotation
Arrow dialog.
3. Create a new 3D annotation
arrow in the Graphics
Window by clicking the New
button.
4. While still in Annot Mode,
Pick the arrow tip location
option in the Pick pulldown.

5. Position the mouse
and press the ‘p’ key.
To manipulate 3D annotation attributes, first
select the item(s) of interest in the list (or while
in Annot Mode, pick them in the graphics
window), then:
To change viewport visibility:
Click on the viewport region to toggle the visibility
in the viewport. Green means visibility is on.
Under Lighting Tab, change surface
characteristics:
Shininess is surface smoothness, intensity is how
much white light in reflected color, and diffusivity is
amount of ambient light reflected.

Under Size Tab, change size:
Arrow size is in global coordinates. Arrow radius,
tip length and tip radius are all in percent of arrow
size.
Note that scaling of the arrows can also be
contolled below and above given value ranges.

Page 375

Under the Location Tab, change location:
The origin can be set by interactive query probe
locations, xyz coordinate, or external force or
moment vector glyphs. For example, for xyz location
- either type appropriate coordinates in the X, Y, and
Z fields or enter a node ID or an element ID. Offset
value moves the arrow backwards.
and orientation:
Buttons: The X, Y, Z orient the arrow parallel to the
axis, Flip reverses 180 degrees, and Normal is
normal to a surface (active only if a surface).
Sliders: Also you can rotate the normal about the X,
Y, or Z. it here.
For the other “Origin by” options appropriate
attributes are presented.

Under the Label Tab, change Label
characteristics:
Type in the arrow label, size it, and color it here.
If the 3D arrow Location was defined as the
location for an interactive query you can
append the interactive query value.
The arrow label can also be defined as an
existing text annotation id. Specify the ID here
and set the text size and color.

SEE ALSO
User Manual: Annot Mode

Page 376

Create Dials

INTRODUCTION
EnSight can display A 2D dial (such as a clock to measure time) tied to a constant variable. These 2D dials overlay
the Graphics window and are not associated with any viewport.

BASIC OPERATION
1. Click Annot in the
Mode Selection Area.
2. Click the Dials icon from the
Mode Icon Bar to bring up the
Annotation dialog.
3. Create a new dial in the
Graphics Window by
selecting a variable in the
Constant variable list and
then clicking the New button.

To manipulate dial attributes, first select the
dial(s) of interest in the list (or while in Annot
Mode, pick them in the graphics window), then:
To change visibility:
Toggle Visible on or off. Note that in Annot Mode
invisible shapes are drawn in a subdued color.
To change whether border is drawn:
Toggle Border on or off.
To change the number of tick marks:
Enter the number of tick marks.
To change the size of the dial:
Enter a value for the dial radius or use the slider.
Values are 0 to 1.

Example:

To change location:
Either select the dial and drag it to the desired
location, or type appropriate coordinates into the
Origin X/Y fields. The origin of a dial is the center.

To delete a dial, click the Delete button.
The Big hand, Little Hand, Value and Background
area is explained on the next page.

Page 377

Attributes for the Big hand
The dial "big hand" points straight up at the minimum value
and has a range specified. If the variable being tracked
exceeds the range the modulus of the variable and the range
is shown.
To change any of the Big hand attributes click the "Big
hand" tab.
To change the minimum value:
Enter the minimum value in the field.
To change the range:
Enter the range in the field.
To change color for the big hand:
Select the desired color from the matrix, enter RGB values
in the fields, or click More... to open the Color Selector
dialog.
Attributes for the Little hand
The dial "little hand" may be visible or not. If visible it is simply
the count of how many rotations the big hand has made. A
value of 0 is straight up and can not be changed.
To change any of the Little hand attributes click on the
"Little hand" tab.
To change the little hand visibility:
Click on the Display toggle.
To modify the Little hand range:
Enter a new range value.
To change color for the little hand:
See instructions under Big hand.
Attributes for Value
The dial may display a value on the dial representing the
variable value or the number of rotations the little hand has
made.
To change any of the value display attributes on the dial
click on the "Value" tab.
To change the value visibility:
Click on the Display toggle.
To change the size of the font:
Enter a font size.
To change the display type:
Set Show as to Revolutions if you wish the value to indicate
the number of revolutions that the Big hand has made or set
to Value if you want to display the variable value.
If you set the Show as to Value you can also set the format
being used by modifying the Format type and the number of
Decimal places.
To change color for the little hand:
See instructions under Big hand.

Page 378

Attributes for the Background
Controls the shading and color of the dial.
To remove the dial background:
Click on the Display toggle. When off no dial background
will be displayed (the dial will be in "wireframe").
To change color for the background:
See instructions under Big hand.

SEE ALSO
User Manual: Annot Mode

Page 379

Create Gauges

INTRODUCTION
EnSight can display a 2D gauge tied to a constant variable. These 2D gauges overlay the Graphics window and are
not associated with any viewport.

BASIC OPERATION
1. Click Annot in the
Mode Selection Area.
2. Click the Gauge icon from the
Mode Icon Bar to bring up the
Annotation dialog.
3. Create a new gauge in the
Graphics Window by
selecting a variable in the
Constant variable list and
then clicking the New button.

To manipulate gauge attributes, first select the
gauge(s) of interest in the list (or while in Annot
Mode, pick them in the graphics window), then:
To change visibility:
Toggle Visible on or off. Note that in Annot Mode
invisible shapes are drawn in a subdued color.
To change whether border is drawn:
Toggle Border on or off.
To change the orientation:
Set the orientation to Vertical or Horizontal.
To change the width/height:
Enter a new width/height value or use the sliders.
Values are 0 to 1.

Example:

To change the variable range:
Adjust the min and max values. If the variable
value being tracked is greater than or equal to the
maximum value, the gauge will be “full”. Similarly,
if the variable value is less than or equal to the
minimum value, the gauge will be “empty”.
To change location:
Either select the gauge and drag it to the desired
location, or type appropriate coordinates into the
Origin X/Y fields. The origin of a gauge is the
lower left corner.

The Gauge level, Value and Background area
is explained on the next page.

To delete a dial, click the Delete button.

Page 380

Attributes for the Gauge level
You can modify the gauge foreground color (the color tracking
the variable value) by:
Click on the Gauge level tab/button.
Select the desired color from the matrix, enter RGB values
in the fields, or click More... to open the Color Selector
dialog.

Attributes for Value
A label may be placed on the gauge to indicate the current
value of the tracked variable.
To change any of the value display attributes on the
gauge click on the "Value" tab/button.
To change the value label visibility:
Click on the Display toggle.
To change the size and location:
Set the font size and the location for the label.
To change the format:
You can set the format to floating or exponential format. For
both formats you can specify the number of decimal places
to display.
To change color for the value label:
See instructions under Gauge level.
Attributes for the Background
Controls the shading and color of the gauge.
To remove the gauge background:
Click on the Display toggle. When off no gauge background
will be displayed (the gauge will be in "wireframe").
To change color for the background:
See instructions under Gauge level.

SEE ALSO
User Manual: Annot Mode

Page 381

Load Custom Logos

INTRODUCTION
EnSight can display bit mapped graphics loaded from disk files. A bitmap can be any image, however, the most
common use is to include a logo or other signature graphic to identify the source of images or animations. Bitmaps
are drawn over all geometric objects in the Graphics Window (at least where the bitmap is opaque), but under all
other annotation entities.

BASIC OPERATION
To load a logo:
1. Select Annot in the Mode Selection
Area
2. Click the Logo icon from the Mode
Icon Bar to open the Annotation
dialog.
3. Click New button and select the
supported image format file using the
File selection dialog which comes up,
and click Okay.
(The supported file formats are listed in
the File Selection dialog under the File
type pulldown.)

To manipulate logo attributes, first select the
logo(s) of interest in the list (or in the graphics
window), then:
To change visibility:
Toggle Visible off or on. Note that in Annot Mode, the logo will not
be completely invisible but will be displayed in a subdued color.
To change location in the graphics window:
Either position the logo interactively by selecting the desired logo
in the Graphics Window (while in Annot Mode) and dragging it to
the desired location, or specify the precise coordinates in the X
and Y fields.
To change size:
Typing the desired scaling factors into the X & Y fields and press
return.
Note that the size of a logo cannot be adjusted interactively.

SEE ALSO
User Manual: Annot Mode

Page 382

Create Color Legends

INTRODUCTION
Every currently active variable has an associated color legend that can be displayed in the Graphics Window. Color
legends provide essential information about images that use parts colored by variable values (color fringes).
Legends are particularly important if the image is to be viewed by others.
Legends are drawn as a vertical or horizontal color bar with associated variable values. The size and position of the
color legend can be changed. This article discusses changing the appearance of color legends using Annotation
mode. To edit the color palette itself (change colors or change the mapping from variable values to colors) see How
To Edit Color Palettes.

BASIC OPERATION
To display a color legend:
1. On the desktop, click the Variable
legend visibility button.

2. Click the variable legend(s) you
wish to display (or not display).
The list contains legends for scalar
variables and for magnitude of vector
variables. The components of vector
variables will become available in the
list if Show Components is toggled on.
More than one legend can be selected
concurrently.
A button is provided to allow you to
easily turn them all off.
You can also easily get to the palette
editor from here.

Note: ( ) indicates legend not currently visible,
(*) indicates currently visible legend.

Page 383

Resize or Reposition Color Legends in Graphics Window
In Annotation Mode, color legends can be selected in the graphics window and then scaled or moved:
1. Make a color legend visible as described above.
2. Click Annot in the Mode Selection area.

Handles (currently selected)

Like other annotation entities, color legends must be selected prior to
performing an operation. A selected color legend has handles surrounding
the color bar colored in the highlight color (typically green). Unselected color
legends have white handles.

3. Select the desired color legend: move the mouse into the
Graphics Window and click the left mouse button anywhere
within the color bar.
4. To move the color legend, place the mouse pointer within the color bar, click
the left mouse button, and drag to the desired location.
5. To resize the color legend, place the mouse pointer over one of the four
corner handles, click the left mouse button, and drag to the desired size.

Manipulating Other Legend Attributes
1. Click Annot in the Mode Selection
Area.
2. Click Legend icon from the Mode
Icon Bar to bring up the Annotation
dialog.
3. Select the legend(s) of interest in the
list (or in the graphics window), then:
To change visibility:
Toggle Visible on or off.
To change color of text and colorbar
outline:
Select the desired color from the matrix,
enter RGB values in the fields, or click
More... to open the Color Selector dialog.
To change legend orientation:
Click the desired Layout (Vertical or
Horizontal).
To change title position:
Click the Title Pulldown and select either
Above (the default), Below, or None.
To change text position:
Click the Values Pulldown and select either
Left/Bottom (the default), Right/Top, or None.
To change legend type:
Click the Type Pulldown and select either Continuous
(the default) or Discrete.
To change text size:
Enter the desired text size and press return.
To change Value label format:
Either select a pre-defined format from the Value format List or enter a new format
string in the Text Format field.
To change location:
Enter values for X & Y (lower left corner) and width and height, and press return.

Page 384

SEE ALSO
How To Edit Color Palettes
User Manual: Annot Mode

Page 385

Manipulate Fonts

INTRODUCTION
EnSight draws all of its text in the graphics window using TrueType fonts. It is capable of reading and drawing most
TrueType fonts and font collections. Under Windows, it is also capable of rendering internationalized multi-byte text in
annotations, provided an appropriate font containing the necessary glyphs is selected.
To ensure portability between platforms, EnSight includes a collection of cross-platform fonts embedded into EnSight.
These include the typefaces: Arial, Courier New, Symbol, and Times New Roman. If a user restricts font usage to
these font families, resulting .els and other files will be portable. If other font families are used, EnSight may substitute
one of these (or other) fonts if it cannot find a match on the target system. EnSight will also read the installed system
fonts on Windows and Power PC-based Macs. The environmental variable CEI_FONTPATH may be set to a list of ':'
(';' on Windows) separated directory names in which EnSight should also look for .ttf and .ttc files. This allows
the user to use their own fonts in EnSight on any platform.
Fonts are always specified in EnSight as a family name and an optional style with a ':' separator. For example,
'Arial:BoldItalic' specifies the Arial family with the styles Bold and Italic applied. Style names of 'Roman', 'Italic',
'Bold' and 'Oblique' (and combinations) are all recognized by EnSight and are mapped against the internal flags in the
TrueType files themselves. The default fonts, styles and sizes used by EnSight can also be set through a collection of
environmental variables:
ENSIGHT_FONT_DEFAULT_SYMBOL
ENSIGHT_FONT_DEFAULT_OUTLINE
ENSIGHT_FONT_DEFAULT_ANNOT
ENSIGHT_FONT_DEFAULT_SYMBOL_STYLE
ENSIGHT_FONT_DEFAULT_OUTLINE_STYLE
ENSIGHT_FONT_DEFAULT_ANNOT_STYLE
ENSIGHT_FONT_DEFAULT_OUTLINE_SCALE

family to be used instead of the symbol font - default = “symbol”
family to be used for ID/axis labeling - default = “Arial”
family to be used for annotations - default = “Times New Roman”
style to be used with the symbol font
style to be used with the outline font
style to be used with the annotation font
specifies the relative scale for the outline font. The value 100.0 is
the default 200.0 is 2x larger, 50.0 is ½ size

The ENSIGHT_FONT_DEFAULT_*_STYLE environmental variables use a numbering scheme for the styles. The
following values may be added together to form the style:
BOLD
1
ITALIC 2
OBLIQUE 4
ROMAN
8
For example, if the user wanted annotations to default to Arial:BoldItalic, the following environmental variables should
be set (Windows syntax):
set ENSIGHT_FONT_DEFAULT_ANNOT=Arial
set ENSIGHT_FONT_DEFAULT_ANNOT_STYLE=3
This selects Arial and BOLD+ITALIC=3. The default font is not recorded in scenario files. Thus, if a scenario file is
generated with these defaults, for the EnLiten user to see the exact same annotations, they would need to set the
same environmental variables and have the same fonts installed on their system. Font changes made with the 
formatting codes (see below) are embedded into the scenario files and do not require the environmental variable
changes for proper display (but do require the same fonts be installed).
Note: under Windows, EnSight uses Times New Roman as the default font for annotations. This font does not contain
a large selection of multi-lingual characters. For users running internationalized versions of Windows, we suggest
that they set ENSIGHT_FONT_DEFAULT_ANNOT to the name of the typeface that best matches their locale. This
allows for natural internationalized text input.

Page 386

BASIC OPERATION
Font selection dialog
In nearly every location where EnSight allows the user to enter
a text string to be used for display (e.g. text annotations, plot
titles, axis titles, etc), it is possible to change the font. It is also
possible to change the font repeatedly in a string. This is done
by inserting a special code into the string that contains the font
name (See Text formatting codes for details). In several
locations in the EnSight GUI, this operation is simplified via the
font selection dialog which lists all the available font family/style
combinations and allows the user to change fonts in the text
field currently being edited
The current font (possibly the default) is selected in the list
when the dialog is opened. The user may change this font to
any other by selecting from this list and clicking 'Insert' or
'Replace'. The 'Insert' button will insert a new font tag and all
text from the current insertion point to the next font string (or the
end of the string) will be displayed in the selected font. The
'Replace' button will replace the current font tag (or the first one
to the left of the insertion point) with the selected font. If no font
tags are in the string to the left of the insertion point, it inserts
one at the start of the string.

To illustrate the use of font capabilities, Text
Annotation will be used:
Clicking the Edit button in Text Annotation, opens the
Text Annotation Editing Dialog allowing the
modification of a text item.
The text to be edited is typed into the scrolling text
field. Note that pressing 'enter' inserts a new line into
the annotation.
To see the results of the edit, click on the 'Update
text' button or check the 'Dynamic update' box.
When dynamic updates are enabled, the annotations
in the main EnSight window are redrawn with every
keystroke.
Note that this option causes EnSight to record every
keystroke into the command stream as well.
The Normal, Subscript and Superscript radio
buttons allow the user to mark sections of the text to
be in super or subscript form by inserting the special
codes   and  into the text stream.
The Store and Recall radio buttons allow the user to
insert the  and  codes into the text
string for saving and recalling a text position on the
screen. (See font formatting codes)
One other thing to note is the Fonts item in the
Special String list. Selecting this will bring up the
Font Selector dialog shown on the previous page.

Page 387

Font formatting codes
The TrueType rendering system supports a number of special embedded codes. These can generally be placed in
most any string displayed in the EnSight graphics window (e.g. plot titles, axis titles, etc). When the text string is
drawn, these special codes are parsed out of the string and they affect any text to the right of the code. In general, the
effects are additive and to turn an effect off, insert another code that sets the feature back to its default value. The
codes are:










XXX






The text is drawn in "normal" mode.
The text is drawn in superscript mode.
The text is drawn in subscript mode.
Change the current font family and/or style. To change just the font family, use
. To change the style only, use . The
special case of  resets the text family and style to the default.
Change the current scaling and/or vertical line offset. To change only the relative
fontsize, use , where 1.0 is the default size of the text. To change
only the vertical offset of the next text, use . For example,
 simulates superscript. The special case of  resets the scale
and vertical offset to 1.0 and 0.0 respectively.
Store the current text position into slot X (x is an integer from 1 to 9).
Recall the current text position from slot X (x is an integer from 1 to 9).
The store/recall mechanism in conjunction with  allows for accurate
repositioning of text. For example, it allows overstrike of text and for the generation
of simultaneous super and subscripts as well as formatted fractions. Note that slot
0 is reserved for the first character in the current line of text.
Insert a single glyph from the "Symbol" font at this position. Note that 3 decimal
digits must follow the  text.
An arbitrary glyph from a font using its Unicode number. The number must be
specified as four hexadecimal digits. For example,  will produce the
copyright symbol (©) if it is available in the current font.
Set the color of the subsequent text. The user may supply up to 4 floating point
values in the range [0.0,1.0] for the Red, Green, Blue and Alpha (opacity) of the
text. The alpha value defaults to 1.0, while other values default to the value to their
left. Note:  changes just the opacity of the text.
Explicitly move to the next line. This is the same as pressing 'enter' in the textfield.
Note that text shown in the Annotation dialog list for text annotations is displayed
with  in place of all new lines.

Page 388

A simple example
The following is an example of a text annotation that utilizes multiple fonts, multiple lines of text, symbols and the
store/recall feature.

The string entered into the Text Annotation Editing
dialog to create this annotation is:
This is dynamically
updated, multi-line
text... A symbol:120
Stored location____________
The first few words are in normal text, followed by a font change and a new line. Midway through the second line, the
font changes again and at the end of that line, it changes back to the default font and style. The third line ends with a
glyph from the symbol font. The last line starts by storing the location of the 'S' character in slot '1'. It then draws
'Stored location' before the  command recalls current output to the 'S' location. Finally, a row of underscores
are drawn that overstrike the words "Stored location".

A more complex example
The following text annotation example illustrates the use of text colors and some scaling and offset options.

The string entered into the Text Annotation Editing dialog to
create this annotation is shown below (note that this is
actually three lines of text, the first is a single, very long line):
A 091
morecomplex093 example
A transparent example
This example begins by drawing an 'A', then scaling up the text while dropping it a bit below the line before drawing a
left brace '['. It then stores off that location and sets up drawing at the original size, but above the baseline. The color
is changed to red and the word 'more' is drawn. The stored location is recalled and a similar operation is done for the
word 'complex' below the baseline. The scale is set to the same as the first brace, the color is reset to white and the
right brace ']' is drawn. To end the line, the scale and offset are reset and 'example' is drawn in blue. The second line
is a blank line. The final line is a simple example of how to make a piece of text partially transparent. Note that the red
object behind the text can been seen through the text.

SEE ALSO
How To Create Text Annotation
User Manual: Annot Mode

Page 389

Configure EnSight
Customize Icon Bars

INTRODUCTION
EnSight uses several sets of icons to group functionality. To suit personal preferences or simplify the interface, the
order of the icons within each set can be changed or icons can be removed altogether (typically eliminating access to
that portion of functionality).
The icon sets correspond to the seven major groupings of function within EnSight: Main Feature (the icons in the
Feature Icon bar) and the six Modes: View, Part, Annot, Plot, VPort, and Frame. By default, EnSight displays
informative text labels underneath each icon in the Mode icon bars. Once the icon functions have been learned,
these can be removed to save space in the icon bar.

BASIC OPERATION
To customize an icon bar:
1. Select Edit > Preferences..., select General User_Interface and click the Modify and Save Icon Layout...
button.

2. Select the desired icon bar from the Which Icon
Bar pulldown.

3. To disable display of the icon help labels, toggle off the Show
Help Labels For Mode Icons button. (Off by default)
To edit, click the left mouse button at the desired location and change the text. Each entry in the list controls one icon
and has the following components:
Menu ID

Internal ID. (Included for potential future usage – do not change).

Button Name

The name of the icon. (Included for potential future usage – do not change)

Visible status

Either ON or OFF.

Order

Icon order within the bar.

Description

Description printed in the Message Area when the left mouse button is clicked and held on the
icon.

Note that changes will not take effect until the next time you run EnSight. To save your changes, click the Save As
Default button and then click Close. To exit the dialog without saving your changes, just click Close.

Page 390

ADVANCED USAGE
The lists presented in the Icon Bar Preferences dialog are stored on disk as text files in the EnSight defaults directory
(located at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at
C:\Users\username\.ensight92 on Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older
Windows, and ~/.ensight92 on Linux, and in ~/Library/Application Support/EnSight92 on the Mac). If you prefer, you
can edit these files directly with any text editor and the changes will take effect during your next EnSight session. The
files are named as follows:
Main Feature

ensight_feat_panel.def

View

ensight_view_panel.def

Part

ensight_part_panel.def

Annot

ensight_annot_panel.def

Plot

ensight_plot_panel.def

VPort

ensight_viewp_panel.def

Frame

ensight_frame_panel.def

See How to Produce Customized Access to Tools & Features for a description of what can be done when you
activate the user-defined toolbox icon.

SEE ALSO
User Manual: Icon Bars

Page 391

Customize Mouse Button Actions

INTRODUCTION
When the mouse pointer is in the Graphics Window, clicking and holding the left mouse button as you drag will
perform the current transformation (e.g. rotate or zoom) as selected in the Transformation Control area. To perform a
different transformation, you have to move the mouse to the Transformation Control area, select the new operation,
and move back to the Graphics Window. To avoid this, you can redefine how the left mouse works as well as map
additional transformation operations onto the middle and right mouse buttons, combinations of mouse buttons, and
double-clicking of mouse buttons.
This customization only effects the mouse usage while in the Graphics Window. The left button is still used for other
user-interface actions.

BASIC OPERATION
To change the behavior of mouse buttons in the Graphics Window:
1. Select Edit > Preferences..., then click on Mouse and
Keyboard

2. Set each click and drag mouse button pulldown (Left,
Middle, Right and combinations of such) as desired.

3. Set the two button click and drag for each mouse.
4. Set the single click action for each mouse button.
5. Set the action for the keyboard ‘P’ key (see below).
5. Set desired Zoom Style.
Automatic slide will zoom based on the direction and distance the
mouse is moved. To the right or up zooms away, while to the left or
down zooms towards. The distance the mouse is dragged
determines the rate of continuous zoom.
Manual drag zooms in the same directions, but only a distance
relative to the distance the mouse is dragged.
6. Click Save To Preference File to save your changes (if you
want these changes to be the default for future sessions of
EnSight) and Close to exit the dialog.
The new settings will take effect as soon as you hit the close
button. If you clicked Save To Preference Files, your changes are
also written to a file and automatically loaded during future EnSight
sessions.

Page 392

Each mouse button (or combination of mouse buttons) can have one of the following associated behaviors:
Selected When this mouse button is clicked and dragged, the operation performed will be the currently
transform action selected function in the Transformation Control area.
Rotate When this mouse button is clicked and dragged, the operation performed will be rotate.
Translate
Zoom
Rubberband
zoom

When this mouse button is clicked and dragged, the operation performed will be translate.
When this mouse button is clicked and dragged, if Zoom Style is Manual Drag then a zoom
displacement will occur, and if Zoom Style is Automatic Slide then a zoom velocity will occur
When this mouse button is clicked and dragged, the operation performed will be a rubberband
zoom.

Rubberband When this mouse button is clicked and dragged, the operation performed will be a rubberband
selection tool selection tool manipulation.
Selected pick
action
Pick part

When this mouse button is clicked, the currently selected pick action (as previously selected
under the pick icon) will be performed.
When this mouse button is clicked, the pick part action will be performed - causing the part under
the mouse to be selected in the main parts list.

Pick cursor tool When this mouse button is clicked, the pick cursor tool action will be performed - causing the
location cursor tool to move to the picked location.
Pick transf. center

When this mouse button is clicked, the pick transformation center action will be performed causing the center of transformation to move to the picked location.

Pick elements to When this mouse button is clicked, the element blanking action will be performed - causing the
blank element under the mouse to be removed.
Nothing

When this mouse button is clicked, no action will be performed.

Note that at least one of the mouse buttons (or combinations) must be set to “Selected transform action”!
Each double-click mouse action or the keyboard ‘P’ key can be set to the following:
Selected pick
action
Pick part

When this mouse button is clicked, the currently selected pick action (as previously selected
under the pick icon) will be performed.
When this mouse button is clicked, the pick part action will be performed - causing the part under
the mouse to be selected in the main parts list.

Pick cursor tool When this mouse button is clicked, the pick cursor tool action will be performed - causing the
location cursor tool to move to the picked location.
Pick transf. center

When this mouse button is clicked, the pick transformation center action will be performed causing the center of transformation to move to the picked location.

Pick elements to When this mouse button is clicked, the element blanking action will be performed - causing the
blank element under the mouse to be removed.
Nothing

When this mouse button is clicked, no action will be performed.

Note that at least one of the mouse buttons, double-click options or the “P” key must be set to “Selected pick
action”!

SEE ALSO
User Manual: Mouse and Keyboard Preferences

Page 393

Save GUI Settings

INTRODUCTION
The default size and position of the EnSight user interface windows was chosen to try to minimize window overlap.
Since some users may have different criteria for window placement, EnSight provides a method for saving this
information.

BASIC OPERATION
You can move and resize windows using the standard window manager operations. Once you have positioned your
windows as desired:
1. Select Edit > Preferences..., select General User Interface and click Save Size and Position of Main
Windows.

The information is saved in your EnSight defaults directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older Windows, and ~/.ensight92 on Linux,
and in ~/Library/Application Support/EnSight92 on the Mac) in the file ensight.winpos.default.
This and many other preference settings can be set and saved, see How To Set and Modify Preferences.

SEE ALSO
User Manual: Save Window Positions under the General User Interface of Prefs.

Page 394

Define and Use Macros

INTRODUCTION
Advanced users of EnSight often find themselves performing repetitive tasks. EnSight’s macro facility lets you save a
sequence of commands and then assign a keyboard key to those commands such that they are executed when the
key is pressed.
Pressing a key assigned to a macro causes the associated command file to be read and executed. Depending on
how it is set up, a macro can execute it’s file in one of three ways:
1. The command file is executed once for each key press. This mode is useful for one-time operations such as cutting flipbook animation on/off or saving an image.
2. The command file repeatedly executes as long as the key is held down. This is useful for operations that are continuous in nature, such as rotating around the Y axis by 5 degrees.
3. Multiple command files execute in a cycle for each keystroke.
Keystroke macros are defined in a text file, macro9.define. Macros can be defined at a site or local level, with local
macros overriding site macros that might be defined for the same key. The macro9.define file (if any) that resides
in the %CEI_HOME%/ensight92/site_preferences/macros directory defines site-level macros, while the
macro9.define file (if any) under the user’s EnSight defaults directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older Windows, and ~/.ensight92 on Linux,
and in ~/Library/Application Support/EnSight92 on the Mac) will define that user’s local macros. Any command files
referenced by macros must be located in these directories as well.
Most of the functions needed to define and edit macros can be found under the Macros tab of the Command Dialog
(File > Command from the Main Menu).

BASIC OPERATION
Creating Macro Command Files
The first step in creating macros is to save the various command sequences that perform the desired actions. This
can be done in several ways.
One way to save commands for a macro is to save off a command file from an Ensight session. See How To Record
and Play Command Files for more information. Be careful as you perform the operations that are saved to the
command file. Superfluous or errant commands will slow down macro operation or cause errors. You may wish to
view the resulting command files with a text editor and possibly make changes.
A second way to create the command file for a macro is to copy commands from the Command Dialog history

Page 395

window:
1. Mark the desired commands by clicking and
dragging in the history window, or by any
combination of clicking and dragging while
holding down the CTRL key.
2. With the cursor over the marked commands, click
the right mouse button to bring up the action
menu, then select "Copy". This will copy the
commands to the system clipboard.
3. Bring up a text editor and insert the commands
using "Paste".
4. When you are finished building your macro
command file, be sure you save it in the site or
local macros directory (see above).

A third way to create a macro command file is by writing/appending them directly to a file from the Command Dialog
history window:
1. Mark the desired commands by clicking and
dragging in the history window, or by any
combination of clicking and dragging while
holding down the CTRL key.
2. With the cursor over the marked commands, click
the right mouse button to bring up the action
menu, then select "Write/append" to file.
3. A File Selection dialog opens. Select or enter the
desired file to save commands to and click Save.
If the file already exists, the selected commands
will be appended, if it does not, it will be created
with the selected commands.

Page 396

Linking macro command files to keys
To link a command file in the macros directory to a key or mouse button:
1. In the Command Dialog "Macros" tab (File >
Command from the Main Menu), click "New".
The New Macro dialog opens.
2. Select or type a key,
3. Check "Repeatable" if you want the macro to be
repeated while the key is held down.
4. Select any modifier keys such as CTRL or ALT.
5. Enter a brief description of what the macro does.
6. Click "Add" to add a command file for the macro.
6. OR click “Add Menu” to add the functionality from
an existing EnSight menu to the macro.
A File Selection dialog opens.
7. Select the desired file and click Save.
Note: you can select a file anywhere on your system,
and if it is not already in the local .macros directory, it
will be copied there.
8. Repeat steps 6 and 7 for macros with multiple
command files.

Page 397

To change an existing macro definition:
1. In the Command Dialog "Macros" tab (File >
Command from the Main Menu), click "Edit".
2. The Edit Macro dialog opens. Change any of the
values in this dialog, then click "Close".
Your changes will not be written to the macro9.define
file until you either click "Save Changes" in the
Command dialog Macros tab, or close the command
dialog and answer "Yes" to the Save Changes query
message.

OTHER NOTES
A common use of tying more than one command file to the same key is to create a toggle. Make the first command
file turn the option on, and the second command file turn the option off. Then tie both of these to the same key. You
will now cycle through the two command files, effectively creating a toggle situation.

SEE ALSO
How To Record and Play Command Files
User Manual: Macros Tab

Page 398

Set or Modify Preferences

INTRODUCTION
Nearly every operation and function in EnSight is initially set to a default value. Preferences allow you to set these
initial values as well as set some default behaviors such as which time step to initially load for transient data, how the
mouse buttons are defined, etc. When EnSight starts, the preference settings are read from the $CEI_HOME/
ensight92/site_preferences directory and then overlaid by the preference settings found in your EnSight defaults
directory (located at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at
C:\Users\username\.ensight92 on Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older
Windows, and ~/.ensight92 on Linux, and in ~/Library/Application Support/EnSight92 on the Mac).

BASIC OPERATION
1. Bring up the Preferences dialog by selecting Preferences
from the Edit pull-down menu.

The following preference categories are available in the Preferences dialog (and will be explained below):
To Set Annotation Preferences:
To Set Color Palette Defaults:
To Set Command Line Preferences:
To Set Data Preferences:
To Set General User Interface Preferences:
To Set Image Saving and Printing Preferences:
To Set Interactive Probe Query Preferences:
To Set Mouse and Keyboard Preferences:
To Set Part Preferences:
To Set Performance Preferences:
To Set Plotter Preferences:
To Set Query Preferences:
To Set User Defined Input Preferences:
To Set Variable Preferences:
To Set View Preferences:
To Set Viewports Preferences:

Page 399

To Set Annotation Preferences:
1. Select Annotation from the Preference
Categories list.
2. Click the “Click Here To Start” button.
3. Click the Select button in the Annot mode
icons and click Deselect All Annotations.
4. Set any attribute, for example line widths to 2
Pixels, text to left justification, etc.
5. You can also define any annotation (text, line,
and logo) and have it be part of your
preferences. Legends can also be part of the
preferences, but these preferences are
independent of the variable tied to the legend,
i.e., the preference file keeps attributes for the
first, second, third, etc. visible legends.
5. Click Save to Preference File to save the
default annotation attributes. If you have
defined any annotations, a pop-up will ask you
if you want to save this annotation as part of
your default or if your intent is to save the
default attributes only.

Page 400

To Set Color Palette Defaults:

1. Select Color Palettes from the Preference
Categories list.

2. Choose to color by RGB or Textures.

3. Toggle on if you want the color legend to
automatically appear when you color a part by a
variable.
4. Toggle on if you want color legends to be
replaced when the current legend is no longer in
use (i.e., no parts are colored by the variable)
and a new variable is in use.
5. Toggle on if you wish the legend ranges to be
updated when time is changed, thus based on
values of variable at the current time.
6. Set the default legend for per element
variables to be constant over the element or to
vary continuously over the element (averages
with neighbors).
7. Set the default legend editing interface to
simple or advanced
8. If you have predefined color palettes, you can
set one of them to be the default by entering the
name or picking one from the list of defined
palettes.
9. To set default legend attributes, click here.
This will bring up the detail editor for color
legends with no legends selected. In the feature
detail editor, set the desired attributes such as
linear/logarithmic scale, and continuous or
banded type.
10. Click here to save the preferences.

Page 401

To Set Command Line Preferences:
A number of command line parameters exist for
EnSight. These parameters can be set in your
preference file so you do not have to specify them on
the start line each time you use EnSight.
1. Select Command Line Parameters from the
Preference Categories list.

2. Select a command line argument.
An explanation of the selected argument will appear
in the dialog.

3. Click here to add the parameter.
It will be placed in the edit area.
If you make a mistake and add an unwanted
parameter, simply highlight it in the feedback area and
delete it.
If additional information is required, a note will be
posted here to help you.
4. If you need to add additional information, add
any text needed into the edit area.
5. Click here to save the preferences.

Page 402

To Set Data Preferences:

1. Select Data from the Preference Categories
list.

2. If you want to specify a path to look for data,
specify it here.
3. You can specify the default binary file type
here.
4. When transient data is loaded into EnSight
you can choose to specify a beginning time
step. If you do not specify a beginning time step,
either the first or the last time step will be loaded
depending on this preference.
5. After successfully reading data into EnSight
you are presented (for most data formats) with a
part loader if this attribute is set to No Parts. If
set to any other attribute the parts specified will
be loaded and displayed without intervention
from the part loader.
Concerns periodic model updating while
EnSight is running - Please Contact CEI Support
regarding this option.
6. The readers shown with a * will show up in the
pull-down for data format in the EnSight data
reader dialog. You can take readers off of the
pull-down list if you toggle the * off (select the
reader in the list).
7. You can specify the default data type by
typing in the exact name of the reader.
8. Click here to save the preferences.

Page 403

To Set General User Interface Preferences:

1. Select General User Interface from the
Preference Categories list.

2. Toggle to show tool tips (balloon help).
3. Toggle to show long part list.
4. Toggle to show Frame mode as an available
mode.

6. EnSight’s command language records part
names or numbers according to this choice.
Recording by name is more portable for using
the command language with a different dataset
since the part numbers do not need to match
up. However, recording by name produces
slightly larger command files.
7. Click Save Above Items To Preference File to
save the GUI items to your preference file.
8. To Modify EnSight’s Icon Layout, click here.
9. To save as a preference the location and size
of EnSight’s windows, click here.

Page 404

To Set Image Saving and Printing Preferences:

1. Select Image Saving and Printing from the
Preference Categories list.

2. Click the “Click Here To Start” button. This
will bring up the Print/Save Image dialog.
3. Modify the attributes you want for your
preference such as the image format.
4. Click here to save the preferences.

Page 405

To Set Interactive Probe Query Preferences:

1. Select Interactive Probe Query from the
Preference Categories list.

2. Click the “Click Here To Start” button. This
will bring up Interactive Probe quick
interaction area.
3. Modify the attributes you want for your
preference such as Report By, and # Items
Displayed.
4. Click here to save the preferences.

Page 406

To Set Mouse and Keyboard Preferences:

This preference allows you to modify the behavior
of the mouse buttons used during EnSight
transformations. Several different actions are
available for the various single click, multiplebutton single click, and double click options. Note,
it is required to set at least one button to “Selected
transform action” (which means that the button is
set to the action as shown in transformation icons
at the bottom of the EnSight dialog - set to rotate
by default). Also, one mouse or the “p” keyboard
key must be set to “Selected pick action”.
1. Select Mouse and Keyboard from the
Preference Categories list.
2. Modify the preference for each of the mouse
buttons (and keyboard ‘P’ key).
Single click actions available are:

Click and drag options are:

And the possible zoom styles are:

3. Click here to save the preferences.
See How To Produce Customized Pop-Up
Menus for a description of what “User defined
menu” is.

Page 407

To Set Part Preferences:

1. Select Parts from the Preferences Categories
list.
2. Click Allow editing part defaults if you want
to be able to edit part defaults when no parts
are selected.
3. Click the “Click Here To Start” button. This
will bring up Part mode in EnSight and deselect
any parts (so you can edit defaults).
4. Modify any part attribute such as line
thickness.
5. Click Save General Part Preferences To File
to save the default visual attributes for parts.
6. If you want to modify creation attributes for
created parts, specify which dialog you want to
use.
7. Set the part type.
8. Modify the attribute. For example, set
subcontours to 3 for contour parts.
9. Click Save Preferences For Part Type
Chosen To File to save the attributes for the
part type edited.
10. Set the options for the Part List display.
11. Save your choices.

Page 408

To Set Performance Preferences:

1. Select Performance from the Preferences
Categories list.
2. To take advantage of pixel saving when
redrawing a window movement, set this
toggle. (Graphics card speed for reading/writing
of pixels needs to be reasonable to use.)

3. To cull duplicate lines in line drawing mode,
set this toggle.
4. To set fast mode to static, toggle on. The
default is off meaning that the fast display
(i.e., bounding box) is only active during
transformations such that the image returns
back to full graphics display when the mouse
buttons are not depressed. In static mode the
fast representation is continuously displayed.
5. To ensure proper display of transparent
geometry, EnSight must sort all the
transparent polygons in the display. This can
be an expensive operation, particularly if
multiple transparent parts are visible. This
option controls when and how surfaces are
sorted.
In “Interactive” mode, sorting is performed
between every redraw of the view. In
“Delayed” mode, sorting is not performed
while the user is interacting with the view
(while the mouse button is held down). NOTE:
Hidden line overlay does not work with either
“Interactive” or “Delayed”. In “Depth peeling”
mode (which is only available on graphics
cards that support the OpenGL Shading
Language) sorting is done by the graphics
card on a per-pixel basis by rendering the
view repeatedly. This mode scales better as
the number of polygons increases and it does
not suffer a performance hit when multiple
parts are transparent. The number of peels
(and hence the number of surfaces to order
properly) is controlled by the “Number of
peels” field.
5. If using point display for fast display mode,
set the point resolution here.
6. If using sparse geometry display for fast
display mode, set the percent of the model to
show here.
(Only used if immediate mode is being used.)

7. EnSight is a client-server architecture
with the possibility that the two processes
are executing on different and possibly
remote machines. Due to this, a general
abort function is not possible. Instead a
timer abort function is available that will
terminate many server operations after a
set amount of time has passed. If you wish
to set this time-out value turn the toggle
on and set the time-out amount (in
seconds).
8. Click here to save the preferences.

Page 409

To Set Plotter Preferences:

1. Select Plotter from the Preferences
Categories list.

2. Click the “Click Here To Start” button. This
will bring up Plotter mode in EnSight and
deselect any plots and curves.
3. Set any attribute, for example line width for
curves, tick marks for axis, etc.
4. Click here to save the preferences.

Page 410

To Set Query Preferences:

1. Select Query from the Preferences
Categories list.
2. Click this toggle on so that once you create
a query it will be automatically plotted.
3. If Auto Plot Queries is toggled on, then you
have the option to check this toggle. If on and
an existing plot uses the same variables, you
query will be added to this existing plot.
Otherwise an new plot will be created.
4. Click the “Click Here To Start” button. This
will bring up the Query quick interaction area
with all query items deselected.
5. Set any attribute, for example Distance Type
and 30 Samples for the Line tool constraint.
6. Click here to save the preferences.

Page 411

To Set User Defined Input Preferences:

1. Select User Defined Input from the
Preferences Categories list.
2. Turn this on to show the macro panel display
3. Toggle to select the default to display a part
list in the graphics window. This is especially
helpful in full screen mode or a VR environment.
4. Turn this on to activate the user defined input
device (ENSIGHT9_INPUT must be set to the
proper device).
5. A Valuator can be used for zoom operations
(like a virtual joy stick), or Position which
simply means to delta movement in the Z
direction will be used.
6. Sets the sensitivity for the zoom operation.
The values for zoom are scaled by this setting,
so values larger than 1.0 will make the inputs
larger while less than 1.0 will make them
smaller.
7. Mixed mode will use the input devices z
rotate directly but use x and y translation values
for x/y rotations. Direct mode will use the
rotation angles from the input device directly
for all three axis.
8. Sensitivity will set a scaling factor for the
rotation values.
9. Click here to save the preferences.

Page 412

To Set Variable Preferences:

1. Select Variables from the Preferences
Categories list.

2. Turn this on if you want to be notified
before a variable is activated.

3. Toggle to select visibility of functions in the
General Functions list of the New Variable
Calculator dialog.

4. Save this notification request and function
visibilities to the preference file by clicking
here.
5. Brings up the dialog for setting extended
CFD settings.
Save these settings by clicking here.

Page 413

To Set View Preferences:

1. Select View from the Preferences
Categories list.

2. Turn on if you want the plane tool to be
shown as a transparent plane, or off if you
want it shown in line drawing mode.
3. There are two offsets employed in EnSight.
This one, hardware offset, is perpendicular to
the monitor screen, and done in hardware if
this toggle is on. This will allow, for example
contour lines to appear closer to the viewer
than their parent part so they are visible no
matter what orientation the part is viewed
from.
The second offset is the display offset. The display offset
can be set in the feature detail editor for line parts such as
contour lines, particle trace lines, vector arrows, and
separation/attachment lines. The display offset is the
distance in the direction of the element normal
(perpendicular to the surface).

4. Select the default viewing orientation.
5. For newer graphics cards leave as
‘hardware’ and EnSight will attempt to use
hardware picking, and if not available will use
software picking. For older graphics cards
with sluggish performance, choose software
picking.
6. Pull down “View” menu and set items
desired.
7. Click here to save the preferences. Caution:
if you save software picking and later change
to a newer graphics card you must change
this back to ‘hardware’ to take advantage of
the new card.

Page 414

To Set Viewports Preferences:

1. Select the Viewports Category.

2. Click the Click Here To Start button.
This will bring up the Viewports quick interaction
area with all viewport items selected.
3. Set any viewport attributes (for example,
background color to blended).
4. Click here to save the attributes set in 2. to
the preference file as defaults for future
sessions.
5. Click her to save the current viewport layout
to the preference file.

SEE ALSO
User Manual: Edit Menu Functions

Page 415

Enable User Defined Input Devices

INTRODUCTION
EnSight offers user defined input devices that have been specifically designed for (but not limited to) typical input
devices used in VR environments. Implementation of these input devices requires adherence to the instructions
outlined in the respective reference files listed below.

BASIC OPERATION
Manual Panel Interface:
1. Select Edit > Preferences..., and click User
Defined Input.
2. Toggle Macro Panel Interface
The Main Graphics window updates the Macro Panel as
defined in the EnSight Defaults Directory (located at
%HOMEDRIVE%%HOMEPATH%\(username)\.ensight92
commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and
Settings\yourusername\.ensight92 on older Windows,
and ~/.ensight92 on Linux, and in ~/Library/Application
Support/EnSight92 on the Mac) as the following file:
hum.define
(If you have not created this file, an example is provided
in:
$CEI_HOME/ensight92/src/udi/HUM/hum.define
on your EnSight Client host system.)

3. Toggle Part Panel Interface (if you desire a
part list in the graphics window).
4. Toggle User Defined Input.
(Detailed steps to implement the User Defined Input
Device are outlined in the file:
$CEI_HOME/ensight92/src/udi/README.v3
on your EnSight Client host system.)

5. Set Zoom Using to the appropriate type of
input device you are using to record zoom
transformations, adjusting the Sensitivity as
needed (i.e., 0 < slower < 1 faster).
6. Set Rotate Using to the appropriate type of
input device you are using to record rotation
transformations, adjusting the Sensitivity as
needed (i.e., 0 < slower < 1 faster).

SEE ALSO
User Manual: “User Defined Input Preferences”

Page 416

Produce Customized Pop-Up Menus

INTRODUCTION
EnSight includes pop-up menus invoked via the right mouse button. The menus can be specific to each mode (i.e.
Part, VPort, Annot, etc), the currently selected parts or other EnSight state. They are written as Python objects that
are dynamically loaded from the EnSight extension repository when EnSight starts up. Menus can realize any
function that can be built on top of command language or Python. Most menus use Python constructs to query
EnSight state and perform customized actions based on that state.
There is a formal mechanism through which EnSight users may add additional, customized menus to the existing
pop-up menus with all of the same capabilities. The mechanism opens up EnSight to specific customization to meet a
particular site or individual user’s needs.

BASIC OPERATION
This section describes the default EnSight menu usage with no additional customization. To use the capability
included with EnSight, simply right click on a part, on some text, or on the background as shown below. By default,
the pop-up menus are tied to the right mouse button single click. This can be changed using options outlined in: How
To To Set Mouse and Keyboard Preferences:. The menus can also be accessed by assigning them to a particular
keystroke as a macro using as outlined in How To Define and Use Macros. The specific menu that is displayed
depends on the current mode, what objects are selected and what object was clicked on. Some examples are shown
here:

Clicking on an annotation
Clicking on a selected part
Clicking on the viewport background

Once the menu has been displayed, you may select from the menu or any of its sub-menus.
Menu targets
In general, the target of the operation is listed at the top of the menu. A special modifier key (‘ctrl’) is used to control
object/part selection. When the menu click is made, a pick operation is performed under the mouse pointer. This pick
returns the selected part or object. If that object is part of the current selection, the selection is not changed and the
Page 417

entire selection is the target of the menu operation. If the object is not part of the current selection, the object
becomes the current selection and again the menu operation is performed on this new selection. The ‘ctrl’ key can
be used to modify this behavior. In normal left mouse button picking, the ctrl key tells EnSight that the picked object’s
selected status should be toggled, without changing the selection status of other objects. In popup menu picking
(right mouse button), the ctrl key tells EnSight not to change the current selection and to target the current selection,
even if the pick operation did not include a selected object. This can be used to more easily bring up the popup menu
operations for objects that are not easily clicked on, or even visible.

ADVANCED USAGE
This section describes how to create custom user-defined menus as explained by How To EnSight extension
mechanism in the Interface Manual. This section assumes familiarity with the Python language, as well as objectoriented programming. Custom pop-up menus have the same capabilities as the built-in menus, the built-in ones are
in fact built on the same interface. For instance, these menus can be specific to an EnSight mode (i.e. Part, VPort,
Annot, etc), the currently selected part types or other EnSight state. Also, customized menus allow the user to display
options, including cascading menus. By default, your custom menus will appear below EnSight’s default list of options
that appear when you right click. The user may also define a key (using the macro facility) to invoke the operation as
noted above.
EnSight includes two well-documented, example Python files to demonstrate the process of createing custom, userdefined pop-up menus. As an exercise to show how to customize EnSight, these two files can be moved from their
existing location to a directory where they will automatically load into EnSight at startup and change EnSight’s
menus.

How menus get loaded
By default EnSight scans the Python files found in subdirectories of the site-specific $CEI_HOME/ensight92/
site_preferences/extensions/user_defined directory and in the user specific EnSight Defaults Directory
(located at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at
C:\Users\username\.ensight92 on Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older
Windows, and ~/.ensight92 on Linux, and in ~/Library/Application Support/EnSight92 on the Mac) under the
extensions/user_defined directory, looking for user-defined tools and menus (specific details of this process
are covered in How To EnSight extension mechanism). When EnSight finds a candidate Python file, it loads it into
a private Python module and calls a “factory” function specified by the menu writer located in the file. The factory
function returns a list of objects that are registered with EnSight. The objects can be user-defined menus, tools and
GUIs, based on the extension class they subclass from. Whenever a pop-up menu is invoked by the user (normally
though the right-mouse button), EnSight will filter the list of registered menu objects, display them as a pop-up menu
and will invoke the run method on any menu selected by user interaction with the menu.
In the next two sections, we walk thought two simple examples of writing custom EnSight user-defined menus.

“Hello world” menu
Shown below is perhaps the simplest example menu entension implementation. It can serve as a template for more
useful menus. This example Python file is included with your EnSight installation in the following folder $CEI_HOME/
ensight92/src/user_defined_ext/ . Copy the entire folder to your user EnSight Defaults Directory (located
at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at C:\Users\username\.ensight92 on
Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older Windows, and ~/.ensight92 on Linux,
and in ~/Library/Application Support/EnSight92 on the Mac) extensions/user_defined/examples folder and
restart EnSight to install the menus. The figure that follows shows the new menu item generated from this Python
code, as well as the console output which is found in the Python window (File>Command, and click on the Python tab
in the resulting window). It also illustrates the directory structure for placing the files into the user specific EnSight
startup path.

Page 418

DocumentsandSettings\username\.ensight92\extensions\user_defined\examples

Shown below is the commented Python code. Notice in particular the block of comment lines starting with
#ENSIGHT_USER_DEFINED_BEGIN and ending with #ENSIGHT_USER_DEFINED_END. These specially formatted
Python comments are what EnSight scans .py files for at startup while looking for extensions. The specify the name
of the function to call when this file is loaded at startup. That (factory) function is responsible for creating instances of
the menu object and returning them to EnSight where they are registered with the pop-up menu handler for future
use.
#
# This comment block is required to identify the file for loading at
# startup by EnSight. The function named by FACTORY= (in this case
# 'ctor' is called by EnSight on startup. Note: the file is loaded
# as a module in EnSight and the path to this file is added to sys.path.
#
#ENSIGHT_USER_DEFINED_BEGIN
#FACTORY=ctor
#ENSIGHT_USER_DEFINED_END
#
# Import the parent class for all user-defined menus and the ensight module
#
import ensight
from ensight.core.menu_extension import menu_extension
#
# Define a menu class, a subclass of the menu_extension class
#
class hello_menu(menu_extension):
#
# Construct the menu with reasonable defaults
#
def __init__(self,name,parent,text="",tooltip="",desc="",icon=None):
menu_extension.__init__(self,name,__file__,1.0)
if (parent): parent.addChild(self)
if (icon): self.setIcon(icon)
self.setText(text)
self.setDesc(text)
self.setTooltip(text)
#
# Method that is called when the menu is selected
#

Page 419

def run(self):
#
# Do whatever operation this menu should do, replace with your own code
#
print "Hello, these parts are selected:"
for part in ensight.query_parts(client=1):
print part[3]
#
# Construct a list of menu objects to be added to the global list of
# user-defined menus
#
def ctor(parent):
list = []
#
# Create the actual menu object, giving it a unique name an
# onscreen name and a text description
#
p = hello_menu("hello_menu",parent,"Hello menu","Menu description")
list.append(p)
return list

Context-sensitve, Hierarchial Menus
Shown below is a more complex menu example. Again, it can be installed in the same manner as described above
and the resulting menus are illustrated in the following image.

This example builds on the previous one. First, it demonstrates that a single Python file can generate as many
menus as it wants. It also demonstrates the ability to define a heirarchy out of those menus. In this example, the
menus themselves have expressed the desire to only be displayed in specific contexts, e.g. when EnSight is in a
specific mode and when a specific type of part has been selected. Finally, several other menu options are set, the
name of the “vendor” for the menu and an icon are specified. More options are documented in the Interface Manual.
The basic file structure is the same as before. There is a header block followed by the various class definitions
followed by the factory function.

Page 420

#
# This comment block is required to identify the file for loading at
# startup by EnSight. The function named by FACTORY= (in this case
# 'ctor' is called by EnSight on startup. Note: the file is loaded
# as a module in EnSight and the path to this file is added to sys.path.
#
#ENSIGHT_USER_DEFINED_BEGIN
#FACTORY=ctor
#ENSIGHT_USER_DEFINED_END
#
# Import the parent class for all user-defined menus and the ensight module
#
import ensight
from ensight.core.menu_extension import menu_extension
#
# Define a "separator" menu class used to put a dividing line between menus
#
class sep_menu(menu_extension):
def __init__(self,name,parent):
menu_extension.__init__(self,name,__file__,1.0)
self.setSeparator(True)
if (parent): parent.addChild(self)
#
# Define a menu class, a subclass of the menu_extension class
#
class part_menu(menu_extension):
#
# Construct the menu with reasonable defaults
#
def __init__(self,name,parent,text="",tooltip="",desc="",icon=None):
menu_extension.__init__(self,name,__file__,1.0)
if (parent): parent.addChild(self)
if (icon): self.setIcon(icon)
self.setText(text)
self.setDesc(text)
self.setTooltip(text)
self.setVendor("John Q. Public")
#
# Method that is called when the menu is selected
#
def run(self):
#
# We are constructing two instances of this class. They differ by
# name. We use the name to perform different operations for each
# of the instances. This could also be done with any other class
# data, including user defined data members.
#
if (self._name == "allpart_menu"):
print "All parts hello!"
else:
print "Model part specific hello!"
#
# Construct a heirarchy of menus. A parent "roll-over" menu and two
# children with a separator between them. These menus use context
# sensitive filtering. The parent is only displayed in EnSight "Part" mode.
# One child is always display and the other is only displayed when the
# currently selected part is a "Model" part. Note: this filtering could
# also be performed by overriding the "validFilter()" method on the menu
# object to perform any custom filtering operation.
#

Page 421

def ctor(parent):
#
# The factory method always returns a list of object to be added.
# In this example, we only return menu_extension subclass instances,
# but the list can include any combination of object subclassed from
# the core_extension class.
#
list = []
#
# Create the parent roll-over menu
#
p = menu_extension("placeholder",None)
#
# Create an icon for the menu (this is optional). In this case, we
# access one of the icons embedded in EnSight itself. See the Qt
# resource management documentation for details.
#
p.setIcon(":/ensight/ens_icn_small")
#
# Set the EnSight mode filter to only display in "Part" mode.
#
p.setMode("Part")
#
p.setText("Simple part tools")
p.setTooltip("Example part tools")
if (parent): parent.addChild(p)
list.append(p)
#
# Create the instance of the part_menu class that should be displayed
# for any part that is selected.
#
m = part_menu("allpart_menu",p,"All part menu","Menu description")
list.append(m)
#
# Add a horizontal separator line between the child menus.
#
m = sep_menu("sep1",p)
list.append(m)
#
# Create an instance of the part_menu class that is only displayed
# when a "Model" part is selected.
#
m = part_menu("modelpart_menu",p,"Model part menu","Menu description")
#
# Set the EnSight part type filter to "Model" parts.
#
m.setPartType("Model")
list.append(m)
return list

Other examples
The example source code shown here is included in the $CEI_HOME/ensight92/src/user_defined_ext/
examples directory, but many other examples exist. The source code to all of the built-in menus is included in the
$CEI_HOME/ensight92/site_preferences/extensions/user_defined directory (and its subdirectories).
Some other example objects are included in $CEI_HOME/ensight92/site_preferences/extensions/
user_defined/Tools/QuickTools/Examples. While these are user-defined tools instead of menus, the
extension mechanisms for both share a large number of common features and techniques that work in one often
work in another. There are a pair of worked tools examples located in the user-defined tool How To Advanced

Page 422

Usage that demonstrate the ability of all user-defined extensions to be able to generate and execute custom
command language and external icon files.
To get the most out of this mechanism, menu developers are encouraged to utilize Python scripts and convert
command language scripts into Python using the provided tools. The Python interface is largely documented in the
Interface manual How To EnSight Python Interpreter.

SEE ALSO
How To Command Language Manual
How To Interface Manual
How To Mouse and Keyboard Preferences
How To Produce Customized Access to Tools & Features

Page 423

Produce Customized Access to Tools & Features

INTRODUCTION
EnSight allows users to define toolbox items, that are accessed by selecting the "User Defined" toolbox feature icon.
These items are collections of custom Python code and command language scripts that perform common operations.
These tools can include full, persistant GUI interfaces and interact with all of the core EnSight state. The mechanism
opens up EnSight to specific customization to meet a particular site or individual user’s needs.
Tool are written as Python objects that are dynamically loaded from the EnSight extension repository when EnSight
starts up. There is a formal mechanism (EnSight extension mechanism) through which EnSight users may add
their own, custom tools.

BASIC OPERATION
The user defined tool icon should be displayed by default. If it is not, it can be turned ON through Edit>Preferences->General User Interface->Modify and save icon layout To access the user-defined
1. Click on the User Defined Tools Icon.
2. The User Defined Tools Window appears.
The EnSight QuickTools are a collection of common
operations that would normally take many steps to
complete in EnSight, packaged in a simpler form.
a) Find the min/max of the selected parts of the colored
variable
b) Calculate the pressure net force and moment and find
center of pressure
c) Use a python calculator
d) Resample transient data to a uniform timestep
e) View alternative EnSight Graphical User Interfaces.
d) Export data in OpenJT format.
f) Import a CSV text file as an EnSight Query.
g) Click on the Presentation Tools to quickly create
output and lanuch the CEI post-processing tools.
h) Submit a bug or support request to CEI and browse
our FAQs.
i) learn how to make your own Python GUI for your
python routines
j) Import an image or movie as an annotation.
k) Modify Case Gold file to include rigid body motion
l) Generate a skybox texture around your data.

tools, click the icon to bring up the dialog and make a selection from the dialog by double clicking.
Page 424

ADVANCED USAGE
This section describes how to create custom user-defined tools as explained by EnSight extension mechanism in
the Interface Manual. This section assumes familiarity with the Python language, as well as object-oriented
programming. Customi tools have the same capabilities as the built-in tools, the built-in ones are in fact built on the
same interface. By default, your custom tools will appear below EnSight’s built-in list of tools that are displayed in the
user-defined tools dialog.
EnSight includes two well-documented, example Python files to demonstrate the process of createing custom, userdefined tools. As an exercise to show how to customize EnSight, these two files can be moved from their existing
location to a directory where they will automatically load into EnSight at startup and change EnSight’s tool list.

How menus get loaded
By default EnSight scans the Python files found in subdirectories of the site-specific $CEI_HOME/ensight92/
site_preferences/extensions/user_defined directory and in the user specific EnSight Defaults Directory
(located at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92\extensions\user_defined\Tools commonly
located at C:\Users\username\.ensight92\extensions\user_defined\Tools on Vista and Win7, C:\Documents and
Settings\yourusername\.ensight92\extensions\user_defined\Tools on older Windows, and ~/.ensight92/extensions/
user_defined/Tools on Linux, and in ~/Library/Application Support/EnSight92/extensions/user_defined/Tools on the
Mac). In the extensions/user_defined subdirectory, looking for user-defined tools and menus (specific details
of this process are covered in EnSight extension mechanism). When EnSight finds a candidate Python file, it loads
it into a private Python module and calls a “factory” function specified by the menu writer located in the file. The
factory function returns a list of objects that are registered with EnSight. The objects can be user-defined tools,
menus and GUIs, based on the extension class they subclass from. A registry of user-defined tools is maintained by
EnSight. It is normally displayed as a tree-list in the GUI noted in the previous section. Applications are free however
to invoke any tool using its run method and tools that implement custom command language may be called directly
from the command parser, even in batch mode.
In the next two sections, we walk thought two simple examples of writing custom EnSight user-defined tools.

“Hello world” tool
Shown below is perhaps the simplest example tool entension implementation. It can serve as a template for more
useful tools. This example Python file is included with your EnSight installation in the following folder $CEI_HOME/
ensight92/src/user_defined_ext/examples. Copy the entire folder to your user specific EnSight Defaults
Directory (located at %HOMEDRIVE%%HOMEPATH%\(username)\.ensight92 commonly located at
C:\Users\username\.ensight92 on Vista and Win7, C:\Documents and Settings\yourusername\.ensight92 on older
Windows, and ~/.ensight92 on Linux, and in ~/Library/Application Support/EnSight92 on the Mac) extensions/
user_defined subfolder and restart EnSight to install the menus. The figure that follows shows the new tool item
generated from this Python code, as well as the dialog it generates. It also illustrates the directory structure for
placing the files into the user specific EnSight startup path.

Page 425

Shown below is the commented Python code. Notice in particular the block of comment lines starting with
#ENSIGHT_USER_DEFINED_BEGIN and ending with #ENSIGHT_USER_DEFINED_END. These specially formatted
Python comments are what EnSight scans .py files for at startup while looking for extensions. The specify the name
of the function to call when this file is loaded at startup. That (factory) function is responsible for creating instances of
the tool object and returning them to EnSight where they are entered in the tool registry for future use.
#
# This comment block is required to identify the file for loading at
# startup by EnSight. The function named by FACTORY= (in this case
# 'ctor' is called by EnSight on startup. Note: the file is loaded
# as a module in EnSight and the path to this file is added to sys.path.
#
#ENSIGHT_USER_DEFINED_BEGIN
#FACTORY=ctor
#ENSIGHT_USER_DEFINED_END
#
# Import the parent class for all user-defined tools and the generic dialog
#
from cei.qtgenericdlg import *
from ensight.core.tool_extension import tool_extension
#
# Define a tool class, a subclass of the tool_extension class
#
class hello_tool(tool_extension):
#
# Construct the menu and set up common information
#
def __init__(self,parent=None):
tool_extension.__init__(self,"hello_tool",__file__,1.0)
self.setText("Hello world tool")
self.setDesc("Say hello to the world from a tool")
self.setTooltip("Say hello to the world from a tool")
if (parent): parent.addChild(self)
#
# We have a PNG icon in the same directory as this file
#
dir = os.path.dirname(__file__)
self.setIcon(os.path.join(dir,"hello_world.png"))
#
# Method that is called when the tool is selected
Page 426

#
def run(self):
#
# Do whatever operation this menu should do, replace with your own code
# In the example, we use the "generic" dialog to display "Hello world!"
#
items = []
items.append(['textval',ITEM_TEXT,"Hello world!","A tooltip..."])
dlg = CeiQtGenericDialog(items,None,"Hello world","Ok",cancel=None)
ret = dlg.doit()
if (ret > 0):
#
# If the user pressed ok, do something...
#
pass
#
# Construct a list of menu objects to be added to the global list of
# user-defined tools
#
def ctor(parent):
list = []
obj = hello_tool()
list.append(obj)
return list

Batch-aware tool with custom command language
Shown below is a more complex tool example. Again, it can be installed in the same manner as described above and
the resulting tool is illustrated in the following image.

This example builds on the previous one. When the tool is invoked, it brings up a more complex dialog that prompts
the user for information including integer parameters and a filename. If the ‘Ok’ button is clicked, it creates a snapshot
of the current rendering and saves it do disk. More importantly, it generates custom command language (shown in the
Command dialog window) that when executed in batch mode will perform the same operation. All user-defined
extensions (tools, menus, GUI and even “core”) automatically extend EnSight command language in this fashion.
The super-classes provide a scaffolding that makes it easy to enforce the separation between interface and function.
For example, the tool Python file could easily be extended to provide an interface to the same functionality as a userdefined menu by adding a menu_extension subclass to the same file. The example uses an icon from the built-in
EnSight icon resources. Finally, this example is “persistent”, that is it stores state (in the case the values entered in

Page 427

the dialog) and uses it to repopulate the dialog. A major advantage of EnSight extensions is that they can store state
and have both private data and method members.
The basic file structure is the same as before. There is a header block followed by the various class definitions
followed by the factory function.
#
# This comment block is required to identify the file for loading at
# startup by EnSight. The function named by FACTORY= (in this case
# 'ctor' is called by EnSight on startup. Note: the file is loaded
# as a module in EnSight and the path to this file is added to sys.path.
#
#ENSIGHT_USER_DEFINED_BEGIN
#FACTORY=ctor
#ENSIGHT_USER_DEFINED_END
#
#
# Import the parent class for all user-defined tools, the ensight module
# and the generic dialog
#
from cei.qtgenericdlg import *
from ensight.core.tool_extension import *
import ensight
#
# Define a tool class, a subclass of the tool_extension class
#
class snapshot_tool(tool_extension):
#
# Construct the tool and set up common information
#
def __init__(self,parent=None):
tool_extension.__init__(self,"snapshot",__file__,1.0)
self.setText("Snapshot the current image")
self.setDesc("Save the current image to a disk file")
self.setTooltip("Save the current image to a disk file")
if (parent): parent.addChild(obj)
#
# Create an icon for the menu (this is optional). In this case, we
# access one of the icons embedded in EnSight itself. See the Qt
# resource management documentation for details.
#
self.setIcon(":/ensight/image")
#
# This is where we store the current command langauge parameters
# We start with some defaults...
#
self._params = {'file':'untitled.png','xsize':640,'ysize':480}
#
# A user-defined method that performs the desired operation taking its
# parameters from a Python dictionary. This method can be called from
# interactive operation or in batch, so it should not display anything.
#
def compute(self,params):
#
# Render and save an image to disk. This is only an example.
# A deeper example can be found in the ensight.core.qtimageutils
# module found in:
# $CEI_HOME/ensight92/site_preferences/extensions/core/qtimageutils.py
#
img = ensight.render(x=params['xsize'],y=params['ysize'])
fname = params['file']
Page 428

#
# The render method returns an EnVe image object, simplifying saving.
#
if (img.save(fname) == 0):
return True
if (img.errstr().find("Unknown file format") >= 0):
fname += ".png"
if (img.save(fname) == 0):
return True
return False
#
# Method that is called when the tool is selected interactively
#
def run(self):
#
# Do whatever operation this tool should do, replace with your own code
# In the example, we use the "generic" dialog to prompt the user for
# and image size and a filename.
#
items = []
items.append(['file',ITEM_FILE,"Filename",
"Name of file to save",self._params['file'],OPT_FILE_SAVE])
items.append(['xsize',ITEM_INT,"Width",
"Width of the image in pixels",self._params['xsize'],10,2048])
items.append(['ysize',ITEM_INT,"Height",
"Height of the image in pixels",self._params['ysize'],10,1536])
dlg = CeiQtGenericDialog(items,None,"Save a snapshot")
ret = dlg.doit()
#
# If the user pressed ok, we will continue.
#
if (ret > 0):
#
# Build a dictionary of output values
#
for key in self._params:
self._params[key] = dlg.getValue(key)
#
# Try to perform the operation
#
if (self.compute(self._params)):
#
# The operation succeeded, so we need to record custom
# command language to place the operation into the journaled
# output.
#
self.cmdRecord("xsize '%d'" % self._params['xsize'])
self.cmdRecord("ysize '%d'" % self._params['ysize'])
self.cmdRecord("file '\""+self._params['file']+"\"'")
self.cmdRecord("compute")
#
# All extensions include the ability to record custom command language
# and play it back. Remember that extensions should be able to play
# back their operations in batch mode. This mechanism allows for an
# extension developer to break GUI interaction and the actual operation
# into two parts.
#
# The cmdExec() method is passed all of the custom command language for
# this tool. Here we use a trick where we assume that the recorded
# command language takes the form of actual Python assignment statements.

Page 429

# We break up the passed line and use the Python 'exec()' method to
# recover the information back into a dictionary.
#
def cmdExec(self,str):
p = str.split("'")
try:
key = p[0].strip()
if (key == 'compute'):
self.compute(self._params)
else:
exec("d = "+p[1])
self._params[key] = d
except Exception, e:
print "Error handling the command:",str,e
#
# Construct a list of tool objects to be added to the global list of
# user-defined tools
#
def ctor(parent):
list = []
obj = snapshot_tool()
list.append(obj)
return list

Other examples
The example source code shown here is included in the $CEI_HOME/ensight92/src/user_defined_ext/
examples directory, but many other examples exist. The source code to all of the built-in tools is included in the
$CEI_HOME/ensight92/site_preferences/extensions/user_defined directory (and its subdirectories,
perhaps most notably the QuickTools directory). Other example objects are included in $CEI_HOME/ensight92/
site_preferences/extensions/user_defined/Tools/QuickTools/Examples. There are a number of
user-defined menu examples included as well. While these may not be tools, the extension mechanisms for both
tools and menus share a large number of common features and techniques that work in one often work in another.
There are a pair of worked tools examples located in the user-defined tool Advanced Usage that demonstrate the
ability of all user-defined extensions to be able to create object heirarchies and to include multiple objects inside of a
single Python module.
To get the most out of this mechanism, menu developers are encouraged to utilize Python scripts and convert
command language scripts into Python using the provided tools. The Python interface is largely documented in the
Interface manual EnSight Python Interpreter.

SEE ALSO
Command Language Manual
Interface Manual
Produce Customized Pop-Up Menus

Page 430

Page 431

Setup For Parallel Computation

INTRODUCTION
Ensight supports shared-memory parallel computation via POSIX threads on all of our supported platforms.

BASIC OPERATION
Configuration
Each executable of EnSight can be configured individually to control the number of threads used.
The following environment variables are used to specify the maximum number of threads that the
executable can use for computation.
ENSIGHT9_MAX_THREADS
The maximum number of threads to use for each EnSight server. Threads are used to
accelerate the computation of streamlines, clips, isosurfaces, and other compute-intensive
operations.
ENSIGHT9_MAX_CTHREADS
The maximum number of threads to use for each EnSight client. Threads in the client are
used to accelerate sorting of transparent surfaces.
ENSIGHT9_MAX_SOSTHREADS
The maximum number of threads to use on the server of server in order to start up server processes in parallel rather than serially.

OTHER NOTES
The number of threads is limited to 2 (per client or server) with a Lite license and 4 (per client or server) with a
Standard license, while the upper limit for a Gold license is 128. EnSight, by default, uses threading according to the
license and the number of processors available and will echo this information out to the console at startup.
....
Detected 2 CPU(s)
ensight92.client using 2 threads.
....
Detected 2 CPU(s)
ensight92.server using 2 threads.
When manually setting these parameters it is a good idea to take into account the number of processors on the
system. In general, you will not see benefit from setting the parameters higher than the number of total processors.
Because the server, server-of-servers and client operate in a pipelined fashion, it is not necessary to limit one in order
to apply more threads to another.
Compute intensive server operations that make use of shared memory parallel computations include isosurface,
clipping, and particle trace computations. Client threaded operations include transparency resort and display list
creation.

Page 432

Setup For Parallel Rendering

INTRODUCTION
EnSight Gold now supports general parallel rendering for increased performance, increased display resolution, and
arbitrary screen orientations. The configuration file format and several examples are described in the User Manual.
Just click the link below to see this information.

SEE ALSO
User Manual: Parallel and Distributed Rendering

Page 433

Miscellaneous
Select Files

INTRODUCTION
Many operations in EnSight (such as loading data) require that you specify a file. EnSight uses a standard file open
dialog that lets you quickly search through directories to find the desired file.

BASIC OPERATION
By default, the File Open dialog opens with the directory from which the EnSight client was started as the current
directory.
The following shows the basic components of the File Open dialog:
The Look in pulldown displays the current directory.
Note that the parent of the current directory is shown
ending with “..” (standard UNIX nomenclature). To
change to a directory, double-click it.

Standard back, up, create, and
listing icons can be used.

The File type pulldown controls the listing of
files in the Files list. You can filter what is
shown based on the selection here
The Files list displays the list of
subdirectories and files contained in the
current directory (possibly modified by the
wildcard in the Filter field). To make a file
the current Selection, click it. To accept a
file and close the dialog, double-click it.
The File field contains the full path name
of the file currently selected in the Files
list. This is the file that will be chosen if
Okay is clicked. Change the selection
either by clicking a file in the Files list
or editing the field directly. Pressing
return will accept the Selection and
close the dialog.

Click to accept the current
Selection and close the
dialog.

Click to cancel the
selection and close the
dialog.

Page 434

INTRODUCTION
Although most attributes of EnSight parts can be edited either through the appropriate Quick Interaction area or the
Part Mode icon bar, full control is provided by the Feature Detail Editors for the various part types. Full control over
variables (e.g. activation, color palette editing, and new variable calculation) is also provided through a Feature Detail
Editor.

BASIC OPERATION
You can open the Feature Detail Editor by either selecting the appropriate item from the Edit > Part Feature Detail
Editors menu or by double-clicking the appropriate part icon in the Feature Icon bar. All Feature Detail Editors (except
the two dealing with Variables – see below) contain the same basic components:
Menu:
File (these items are only available for the Variables Feature
Detail Editor – see below)
Edit
Select All: Select all parts listed in the dialog’s parts list
Copy: Make a copy of the selected part(s)
Delete: Delete the selected part(s)
Immediate Modification: If on, all changes in the dialog have
an immediate effect. If off, the Apply Changes button at the
bottom must be clicked to apply your changes (good for
batching several expensive changes).

List of variable/part icons; click to change to the desired
Feature Detail Editor type.
Parts list of the current Feature Detail Editor type; lists only
those parts of the current type. (For example, the contour
Feature Detail Editor is shown and only the current contour
parts are listed.)
Description of the currently selected part in the parts list. Click
to type, make changes, and press return.
Creation Attributes section. This section (which is missing for
Model parts) is unique to the Feature Detail Editor type and
controls part-specific attributes (e.g. the isovalue of an
isosurface).
The remaining sections (General, Node/Element/Line, and
Displacement) control attributes common to all part types. See
How To Set Attributes for more information.
Click to Close the Feature Detail Editor dialog.
Click to Create a new part based on the attributes as currently
set and with parent part(s) as selected in the Main Parts list.
Click to change the parent part(s) of the selected part(s). The
new parent part(s) must be selected in the Main Parts list.

Click to apply any changes you have made (only
active when Immediate Modification is toggled off
in the Feature Detail Editor Edit Menu).

Page 435

The Feature Detail Editor for variables is different from the part Feature Detail Editors:
1. To open the Feature Detail Editor for Variables either
select Edit > Variables Editor... or double-click the Color
icon in one of the modes (such as Part mode).

Menu:
File
Save Selected Palette(s)...: Write palettes for selected
variables to a disk file
Save All Palettes...: Write palettes for all variables to a disk
file
Restore Palette(s)...: Load palettes from a disk file
Edit
Select All: Select all parts listed in the dialog’s parts list
Immediate Modification: If on, all changes in the dialog have
an immediate effect. If off, the Apply Changes button at the
bottom must be clicked to apply your changes (good for
batching several expensive changes).

List of available variables. Click to select a variable.

Buttons to control variable activation/deactivation. See How
To Activate Variables for more information.

The Edit palette... button will bring up a dialog showing the
palette information for the variable. See How To Edit Color
Palettes for more information.

Page 436

The Feature Detail Editor for variable Calculator is also different from the part Feature Detail Editors:
1. To open the Feature Detail Editor for variable Calculator click
the Calculator icon in the Feature Icon bar.

Variable Calculator section. See Variable Creation in the
User Manual for more information.

SEE ALSO
Most of the creation attributes for parts can also be set in the Quick Interaction area for the part type. See the How To
article for the desired part type for more information.
Page 437

Feature Icon Bar
Solution
Time

User
Defined
Tools

Keyframe
Animation

Flipbook
Animation

Query/
Plot

Variable
Calculator

Contour

Interactive
Query

Particle
Traces

Clip

Isosurface

Vector
Arrows

Profile
Plot

Subset
Parts

Separation/
Attachment
Line

Vortex
Core

Elevated
Surface

Shock
Region/
Surface

Developed
Surface

Material
Parts

Boundary
Layer

Tensor
Glyph

Extrusion

Point
Part

Transformation Control Icons
Rotate

Zoom

Translate

Selection ResetTools &
Tool
Viewports

Rubber
Band
Zoom

Transformation
Editor

Color/Transparency
Visibility in Viewport

Store/Recall
last View

Fit in Window

Undo last
transformation

Global Toggle, Tool, and Other Desktop Icons

Part Mode
Visibility

Tool Tip Help

Look Down Axes

Pick Action

Select Tool

Shaded

Cursor Tool

Hidden Line

Line Tool

Highlight Selected

Plane Tool

Vport Mode

Axis Triad

Animation Record

Bounding Box

Legend

Fast Display

Info

Frame Mode

Annot Mode

Line Width

Visibility

Axis Visibility

Text Creation

Element Visual Rep.

Color

Color

Line Creation

Displacement

Layouts

Line Width

Logo Import

Symmetry

Create

New

Legend Attributes

Elem/Node Labels

Move Forward

Part Assignment

Node Rep.

Move Back

Special Settings

Failed Elements

Lighting

Comput. Symmetry

Element Blanking

Border

Axis

Location

Origin Orientation

Shaded
Hidden Line
Auxiliary Clipping
Fast Display Rep.

Special Settings

Delete

Plot Mode
Visibility
Plotter

Transform/Define

Part Bounds

Select All

Select All

Delete

Delete

Select All

Axis
Curve
Select All
Delete

Page 438

A

B

C

D

E

F

G

H

I

Numerics
2D shapes
annotation 373
3D arrows
annotation 375

C

L

M

N

O

P

Q

R

S

D

E

F

G

H

I

J

K

L

M

N

O

T

U

V

W

X

Y

Z

Y

Z

-ctx 22
-custom 22
-dconfig 24
-delay_refresh 22
-display_list 24
-double_buffer 25
-extcfd 22
-externalcmdport 22
-externalcmds 22
-fg 25
-fn 25
-font 25
-frustrum_cull 24
-gdbg 24
-gl 24
-glconfig 24
-glsw 24
-gold 22
-h, -help, -Z 24
-hc 25
-iconlblf 23
-inputdbg 24
-iwd 24
-localhostname 22
-maxoff 24
-multi_sampling 24
-multi_sampling_sw 24
-nb 24
-ni 23
-no_delay_refresh 22
-no_display_list 24
-no_file_locking 24
-no_frustrum_cull 24
-no_multi_sampling 24
-no_occlusion_test 25
-no_prefs 24
-no_start_screen 24
-no_stencil_buff 25
-norm_per_poly 24
-norm_per_vert 24
-num_samples 24
-num_samples_st 24
-occluson_test 24
-ogl 24
-p 22
-ports 23
-prdist 23
-range10 24
-readerdbg 24
-rsh 23
-sc 23
-scaleg 24
-scalev 24
-security 23
-silent 24
-single_buffer 25
-slimtimeout 24
-smallicons 23
-smallscreen 23
-sort_first 25
-sort_last 25
-sos 23
-soshostname 23
-standard 23
-stderr 24
-stdout 24
443
-stencil_buff 25

C
calculator 275
Camera
viewing viewport through 160
camera
look-at 129
look-from 129
look-from point 129
projection 125
specifying for povray 117
virtual, zooming 121
case
adding 53
deleting 55
part, display by 55
reading 52
replacing 55
viewport visibility 56, 138
CEI, Inc. 6
center of transformation
picking 156
CFD variables 282
client/server overview 10
clip
animation 351
auxiliary clipping 132
box 222
general quadric 234
grid 220
IJK 225
line 214, 236
plane 217, 244
quadric 223
revolution of 1D part 233
revolution tool 232
RTZ 230
XYZ 228
Z clipping 127
clipping
plane
using 3 node ids 218
collaboration 31
color
background 135
default 315
legend 383
part 314
selector 154
variable palette 285
command file
play 96
record 95
command line options 22
client
-ar 22
-batch 24
-bbox 24
-bg 25
-box_resolution 24
-c 22
-case 22
-cm 22
-collab_port 22
-ctarget 24

B
background
color 135
image 135
batch mode 24
bitmap logo 382
blanking
elements 269
Block Continuation
using 79
BMP
output 101
border representation 322
boundary layer variables 283
box
B

K

clip 222
tool 174

A
acrobat reader 5, 7
activating variables 273
Animated GIF
output 101
animation
flipbook 351
hints and tips 361
keyframe 355
mode shape 253
particle trace 365
recording to video 364
transient data 348
annotation
2D shapes 373
3D arrows 375
color legend 383
dials 377
fonts 386
environment variables 386
formatting codes 388
gauges 380
line 371
logo 382
preferences 400
text 367
Apple Quicktime
output options 103
archive
restore 93
save 92
arrows, vector 238
attachment line 261
attributes
displacement 328
general 326
IJK Axis Display 328
node, element, line 327
part 324
automatic connection 12
on Unix systems 18
on Windows systems 18
auxiliary clipping 132
AVI
output 100
Axi-symmetric extrusion 244

A

J

P

Q

R

S

T

U

V

W

X

Page 439

A

B

C

D

E

F

G

H

I

-swd 24
-time 24
-timeout 23
-token_try_again 23
-token_wait_for 23
-token_wait_until 23
-unmapdd 25
-v 23
-version 23
-writerdbg 24
-X 25
client examples 25
preferences 402
server
-c 26
-ctarget 26
-ctries 26
-ether 26
-gdbg 26
-h, -help 26
-maxoff 26
-pipe 26
-ports 26
-readerdbg 26
-scaleg 26
-scalev 26
-security 26
-sock 26
-soshostname 26
-time 26
-writerdbg 26
server examples 26
sos
-c 26
-cports 26
-ctarget 26
-ctries 26
-ether 26
-gdbg 26
-h, -help 26
-maxoff 26
-pipe 26
-ports 26
-readerdbg 26
-rsh 26
-scaleg 26
-scalev 27
-security 27
-sock 27
-soshostname 27
-sports 27
-time 27
-writerdbg 27
sos (server-of-servers) examples 27
computation
setup for parallel 432
computational symmetry 336
cone
clip 223
tool 181
connection
automatic 12
automatic on Unix systems 18
automatic on Windows systems 18
collaboration 31
contacting CEI 6
context
A

B

C

D

E

F

G

J

K

L

M

N

O

P

Q

D
data
discrete 254
ens_checker 46
experimental 254
measured 254
preferences 403
reading 36
dataset
information 313
querying 313
reading 36
deactivating variables 274
default color 315
delete
frame 151
part 321
plotter 311
viewport 140
Desktop 10
developed surface 247
dials
annotation 377
discrete data 254
displacement
server-side 252
displacements 251
display remotely 143
displaying stereo 155
distance query 297
documentation
acroabat reader 5
online use 5
printing 6, 7
use of How To 7
E
editing features
detail editor 435
element
blanking 269
failed 267
labels 329
query 292
representation 322
elevated surface 243
email address 6
ens_checker 46
ensight8
start-up options 22
I

J

K

L

M

N

O

P

S

T

U

V

W

X

Y

Z

ENSIGHT8_MAX_CTHREADS 432
ENSIGHT8_MAX_SOSTHREADS 432
ENSIGHT8_MAX_THREADS 432
ENSIGHT8_READER 72
EnVideo output 101
Environment Variables 28
environment variables
CEI_ARCH 29
CEI_CONTROLLER_KEY 29
CEI_DISABLE_PBUF 28
CEI_FONT_GLYPHCACHESIZE 28
CEI_FONT_NOSYSTEMFONTS 28
CEI_FONTPATH 28
CEI_HOME 29
CEI_INPUT 30
CEI_PDFREADER 29
CEI_PIXELFORMAT 28
CEI_PIXELFORMAT_ST 28
CEI_PYTHONHOME 29
CEI_RSH 29
CEI_TRACKD_DEBUG 30
CEI_TRACKER_KEY 30
CEI_UDILPATH 29
CVF_NO_WM_OVERRIDE 28
DISPLAY 29
ENSIGHT_FONT_DEFAULT_ANNOT
28
ENSIGHT_FONT_DEFAULT_ANNOT_S
TYLE 28
ENSIGHT_FONT_DEFAULT_OUTLINE
28
ENSIGHT_FONT_DEFAULT_OUTLINE
_SCALE 28
ENSIGHT_FONT_DEFAULT_OUTLINE
_STYLE 28
ENSIGHT_FONT_DEFAULT_SYMBOL
28
ENSIGHT_FONT_DEFAULT_SYMBOL
_STYLE 28
ENSIGHT_NAGLE 29
ENSIGHT_PATHREPLACE 29
ENSIGHT_PICK_SCALE 28
ENSIGHT8_COLLABHUB_SPAWNDEL
AY 28
ENSIGHT8_FIXED_FONT_SIZE 28
ENSIGHT8_HUB_APP 28
ENSIGHT8_HUB_ARGS 28
ENSIGHT8_HUB_CONNBACKHOST 28
ENSIGHT8_HUB_HOST 28
ENSIGHT8_HUB_OUTPUTFILE 28
ENSIGHT8_INPUT 30
ENSIGHT8_MAX_CTHREADS 29
ENSIGHT8_MAX_SOSTHREADS 29
ENSIGHT8_MAX_THREADS 29
ENSIGHT8_READER 30
ENSIGHT8_READER_GUI 30
ENSIGHT8_RENDERER_HOSTS 28
ENSIGHT8_RES 29
ENSIGHT8_SERVER_HOSTS 29
ENSIGHT8_SOCKBUF 29
ENSIGHT8_UDMF 30
ENSIGHT8_UDW 30
ENSIGHT8_WORKER_APP 28
ENSIGHT8_WORKER_ARGS 28
ENSIGHT8_WORKER_CONNBACKHO
ST 28
443
LSB_MCPU_HOSTS 29

restore 110, 115
save 110, 115
contour 198, 289
copy (part) 316
created variables 275
creating parts 191
cursor tool 164
Custom Access to Tools & Feautres 424
customize
icon bars 390
mouse buttons 392
window positions 394
Customizing Pop-Up menus 417
cut (part) 320
cylinder
clip 223
tool 177

H

R

Q

R

S

T

U

V

W

X

Page 440

Y

Z

A

B

C

D

E

F

G

H

I

PATH 29
TMPDIR 29
experimental data 254
Extent Bounds 157
extract (part) 319
extracting
boundary layer variables 283
separation/attachment lines 261
shock surfaces/regions 263
vortex cores 259
Extrusion 244

E

F

N

O

P

Q

H

I

J

K

L

M

S

T

U

V

W

X

Y

Z

Y

Z

O
online documentation use 5
orthographic projection 125
output formats
Animated GIF 98
Apple Quicktime 98
AVI 98
EnVideo 98
JPEG 98
MPEG1 98
MPEG2 98
MPEG4 98
PNG 98
PostScript 98
POVRAY 98, 116
PPM 98
RGB(Silicon Graphics) 98
TIFF 98
XPM 98
overview 10
client/server architecture 10
graphical user interface 10
parts concept 10
P
palette
editing 285
preferences 401
parallel computation
configuration 432
setup 432
parallel rendering
setup 433
part
attributes 324
box clip 222
clip plane 217, 244
clips 213
color 314
contour 198, 289
copy 316
creation 191
cut 320
delete 321
developed surface 247
displacements 251
element labels 329
elevated surface 243
extract 319
group 317
IJK clip 225
introduction 191
isosurface 200
isovolume 202
line clip 214, 236

M
macros 395
Manage Views 162
Manipulate Fonts 386
map textures 338
material part 265
measured data 254
merge (part) 318
Min/Max Variable Tracks 204
mode shapes 253
Model Axis 157
Model Extent Bounds 157
mouse
buttons, customizing 392
preferences 407
MPEG
output options 102

G

R

N
Network Ports Used 20
Client/Server Mode 20
Collab Hub 20
Distributed Renderer 21
External Commands 20
Server of Server Mode 20
node
labels 329
query 291
Node Tracks 204
not loaded representation 322

L
labels
element 329
node 329
legend, color 383
light source
attributes 142
location 142
lighting
attributes 142
model 326
line
annotation 371
clip 214, 236
tool 160, 166, 189
logo annotation 382
look-at 129
look-from 129

I
icon bar
customize 390
icons
reference 438
IJK
changing step refinement 226
clip 225
interactive plane sweep 226
query 292
image output 98
preferences 405
input devices
defining 416
interactive
D

M

K
keyboard macros 395
keyframe animation 355
Record 360
Run From/To 359
Save and Restore 361
Speed/Actions 357
Tips 361
Transient 360
Viewing Window 358

H
hidden line overlay 123
hidden surface drawing 123

C

L

J
JPEG output 102

G
gauges
annotation 380
general quadric clip 234
general user interface
preferences 404
geometry
file 36
save in EnSight Gold format 106
save in VRML format 106
grid clip 220
group (part) 317

B

K

clipping
IJK 226
line 215
plane 217
quadric 223
RTZ 230
XYZ 229
isosurfaces 201
particle traces 207
probe preferences 406
query 294
isosurface
animation 201, 351
creation 200
interactive 201
isovolume 202
creation 202

F
failed elements
removing 267
using with user-defined API 268
fast display mode 126
fax number 6
feature angle representation 322
feature detail editor 435
file selection 434
flipbook
animation 351
transient data animation 348
font manipulation 386
environment variables 386
formating codes 388
frame
assigning parts to 147
attributes 150
creating 146
deleting 151
repositioning 148
selecting 147
transform reset 149
full representation 322

A

J

N

O

P

Q

R

S

T

U

V

443
W

X

Page 441

A

B

C

D

E

F

G

H

I

map textures 338
material 265
merge 318
node labels 329
particle trace 204
point part 271
preferences 408
profile 246
quadric clips 223
query 293
revolution of 1D part clip 233
revolution tool clip 232
RTZ clip 230
save to disk file 106
selection 332
separation/attachment line 261
shock surfaces/regions 263
subset 248
symmetry
computational 336
visual 335
tensor glyphs 249
texture mapping 338
transparency 331
vector arrows 238
vortex core 259
XYZ clip 228
Part Bounds Display 139
Particle Trace Min/Max Variable Track 204
Particle Trace Node Tracks 204
particle traces
animation 365
creating 204
interactive 207
pathlines 209
streaklines 206
surface restricted 208
parts concept 10
performance
preferences 409
periodicity 335
perspective projection 125
phone numbers 6
pick
center of transformation 156
cursor tool 164
line tool 167
look-at point 131
part 333
plane tool 170
plane clip 217, 244
Plane tool 169
plotter
anatomy 305
attributes 305
create 306
delete 311
moving/resizing 306
preferences 410
selecting 306
visibility 306
PNG
output options 102
point
query 291
point part 271
Pop-Up menus
A

B

C

D

E

F

G

H

J

K

L

M

N

O

P

Q

Q
quadric clip 223
query
dataset 313
element 292
IJK 292
interactive 294
node 291
over distance 297
part 293
point 291
preferences 411
Quicktime
output options 103

K

L

M

N

T

U

V

W

S
save
command file 95
context 110, 115
geometry 106
image 98
keyframe animation 361
POVRAY 116
preferences 399
scenario 112
session (archive) 92
viewing parameters 144
scale 120
scenario
save 112
selecting
colors 154
elements to blank 269
files 434
parts 332
selection tool 186
element blanking 187
for subset parts 248

R
reading
Advanced Interface 40
Advanced Interface/Load All 37
block continuation 79
data (introduction) 36
ens_checker 46
ensight_reader_extension.map file 39
File->Open... 36
new data without quitting 55
Quick method 36, 37
server of servers 59, 66, 156
transient data 57
Two-Step method 40
user defined data reader 72
reference
J

S

X

Y

Z

Y

Z

icons 438
rendering
setup for parallel 433
representation
border 322
bounding box 322
feature angle 322
full 322
non visual 322
reset
frame transform 149
transformations 152
Resources
another sos casefile example 89
client specification 85
client/server example 87
collabhub 86
how to specify 85
prdist example 90
sample 84
simple sos example 87
sos 86
sos casefile example 88
sos example 87
using 84
restart
session (archive) 93
without quitting client 55
restore
context 110, 115
keyframe animation 361
session (archive) 93
viewing parameters 144
result file 36
revolution of 1D part clip 233
revolution tool 183
clip 232
Rigid Body Transformations
saving 109
rotate 120
Rotational extrusion 244
RTZ
clip 230

customizing 417
Ports Used 20
Client/Server Mode 20
Collab Hub 20
Distributed Renderer 21
External Commands 20
Server of Server Mode 20
PostScript output 100
POVRAY 116
output 100
PPM / PGM / PBM
output options 103
preferences 399
annotation> 400
color palettes 401
command line 402
data 403
general user interface 404
icon bar 390
image saving/printing 405
interactive probe 406
macros 395
mouse and keyboard 407
part 408
performance 409
plotter 410
query 411
user defined input 412
variables 413
view 414
window positions 394
printing
documentation 6
images 98
probe query 294
profile plot 246

I

R

O

P

Q

R

S

T

U

V

W

443
X

Page 442

A

B

C

D

E

F

G

H

I

zooming 186
separation line 261
Server of Servers
using 59, 66, 156
server-side displacement 252
setup for parallel computation 432
setup for parallel rendering 433
SGI RGB
output 103
shaded surface drawing 123
shock
surface/region 263
solution time 256
recording animation 257
sphere
clip 223
tool 179
spline
attach plane clip 219
camera origin on 160
curve line type 311
over distance queries 299
Spline Tool 189
starting
automatically 12
options 22
stereo display 155
subset parts 248
pick elements 248
selection tool 248
surface of revolution tool 183
surfaces, developed 247
symmetry
computational 336
visual 335

B

C

D

E

F

K

L

M

N

O

P

Q

H

S

T

U

V

W

J

K

L

M

N

Y

Z

Y

Z

X
XPM output 104
XYZ
clip 228
interactive plane sweep 229, 230
Z
Z clipping 127
zoom 120
rubberband 120
to region 186
using selection tool 186

V
variable
activation 273
and cases
boundary layer 283
calculator 275
color palette 285
common CFD 282
deactivation 274
environment 28
preferences 413
vector arrows 238
density 239
view
preferences 414
viewport
2D or 3D 137
attributes 137
background image 135
camera projection 125
case visibility 138
color 135
creating 133
deleting 140
lighting attributes 142
Part Bounds Display 139
part display 138
repositioning 134
resetting 152
saving viewing parameters 144
standard layouts 133
tracking 137, 159
viewport tracking 137
Views
manage 162
Virtual Reality setup 433
I

X

W
window positions, customizing 394
working variable (default color) 315

U
unrolling surfaces 247
User defined
access to tools and features 424
user defined
data reader 72
input devices 416
input preferences 412
Using Block Continuation
Block Continuation 79
Using Resources
Resources 84
Using Server of Servers
SOS 59

G

R

visual representation 322
vortex cores 259
VR setup 433
VRML 106

transformations
frames 148
resetting 152
rotate 120
scale 120
translate 120
zoom 120
transient data
animation 348
reading 57
setting current time 256
stepping through 256
translate 120
Translational extrusion 244
transparency 331
TrueType fonts 386

T
tensor glyph parts 249
text annotation 367
texture mapping 338
threads
ENSIGHT8_MAX_CTHREADS 432
ENSIGHT8_MAX_SOSTHREADS 432
ENSIGHT8_MAX_THREADS 432
TIFF output 104
time
stepping through 256
tools
box 174
cone 181
cursor 164
cylinder 177
line 160, 166, 189
Plane 169
resetting 152
selection 186
sphere 179
surface of revolution 183
traces
animation 365
creating 204
interactive 207
pathlines 209
streaklines 206
surface restricted 208
tracking 137
tracking in viewports 159
A

J

O

443
P

Q

R

S

T

U

V

W

X

Page 443



---

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.3
Linearized                      : Yes
Page Count                      : 443
Page Mode                       : UseOutlines
XMP Toolkit                     : XMP toolkit 2.9.1-13, framework 1.6
About                           : uuid:9848510f-2349-4bac-a974-f3441acb26f1
Producer                        : Acrobat Distiller 6.0.1 (Windows)
Creator Tool                    : FrameMaker 7.1
Modify Date                     : 2011:01:13 17:46:54Z
Create Date                     : 2011:01:13 17:46:54Z
Document ID                     : uuid:0c42cb1b-a875-4764-8d65-c285a3cd1aaa
Format                          : application/pdf
Title                           : HowTo.book
Creator                         : ensight
Author                          : ensight

EXIF Metadata provided by EXIF.tools