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QUICK REFERENCE GUIDE 
 i 
 
Quick Reference Guide 
By Bryan A. Ross 
Published by 
 
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QUICK REFERENCE GUIDE 
 i 
 TABLE OF CONTENTS 
Table of Contents 
CREO ELEMENTS/DIRECT INTRODUCTION 
Historical Overview ................................................................... ii 
Direct Modeling in Creo ........................................................... iii 
Creo Elements/Direct New Feature Highlights ...................... iv 
 
MODELING 
Interface Introduction ........................................................... 1-3 
 Interface Summary ..............................................................1 
 Files, Ribbons, and Toolbars ..............................................2 
 Right-Hand Rule...................................................................2 
 Dialogue Boxes ....................................................................3 
 Calculator .............................................................................3 
 Workplanes ..........................................................................4
 Real and Construction Geometry .......................................4 
Basic Modeling .................................................................... 5-15 
 Catch, 2D CoPilot, Lock and Keyboard ..............................5 
 Modify 2D and Relative Measurement ..............................6 
 Putting it all Together ..........................................................6 
 Selecting Regions ................................................................7 
 3D Copilot and Reference Cones .......................................7 
 Pull ........................................................................................8 
 Selection ..............................................................................9 
 Blends and Chamfers....................................................... 10 
 Moving and Pulling Faces ................................................ 11 
 Stretch Face, Edge, and Offset ........................................ 12 
 Taper Faces ...................................................................... 13 
 Cut, Copy, and Paste Faces ............................................. 13 
 Punch, Stamp, and Section ............................................. 14 
 Shell and Imprint .............................................................. 14 
 Boolean Operations .......................................................... 15 
 Mirror, Scale, Align, and Merge ....................................... 15 
Advanced Modeling ........................................................ 16-18 
 Freeform Modeling ........................................................... 16 
 Splines, 3D Curves and Points ........................................ 16 
 Projected Profiles ............................................................. 17 
 3D Surfacing Tools ........................................................... 17 
 Features and Patterns ..................................................... 18 
 
MODULES 
Machining ............................................................................... 19 
Surfacing ................................................................................. 20 
Basic Sheets ........................................................................... 21 
 
 
ASSEMBLIES 
Building Assembly Structures ............................................... 22 
Containers .............................................................................. 23 
Copy, Share, and Instancing ................................................. 23 
Advanced Assemblies .......................................................24-25 
 Clipping Planes ................................................................. 24 
 Stock/Finish ..................................................................... 24 
 Coordinate Systems ......................................................... 24 
 Configurations .................................................................. 25 
 Explosions ......................................................................... 25 
 Clash Analysis ................................................................... 26 
 
 
ANNOTATIONS 
Annotation Application .................................................... 27-29 
 Introduction....................................................................... 27 
 Drawing Structure ............................................................ 27 
 Template Browser ............................................................ 27 
 Starting Drawings and Views ........................................... 28 
 Placing and Updating Views ............................................ 29 
 Adding Dimensions, Text, and Objects ........................... 30 
 Sketching Geometry ......................................................... 31 
 BoM Tables ....................................................................... 31 
 Printing .............................................................................. 31 
3D Documentation Application ....................................... 32-34 
 Introduction....................................................................... 32 
 Setup ................................................................................. 32 
 Annotate ............................................................................ 33 
 Display ............................................................................... 33 
 Modify with Dimensions ................................................... 33 
 BoM ................................................................................... 34 
 Group ................................................................................. 34 
 Template Browser ............................................................ 34 
MODEL MANAGER 
Introduction ........................................................................... 35 
Model Manager Breakdown ................................................... 36 
Search and Load ................................................................... 37 
Save ........................................................................................ 38 
Conflict Resolution ................................................................. 38 
Bill of Material Editor ............................................................39 
Versions and Inseparable ...................................................... 39 
 
 
APPENDIX A — SUPPORT 
Platform Support .................................................................. 40 
Technical Support ................................................................... 41 
 
 
APPENDIX B — SHORTCUTS 
Creo Elements/Direct Shortcuts ........................................... 42 
 
 
APPENDIX C — STRUCTURE BROWSER ICONS 
Structure Browser Icons ......................................................... 43 
 
 
APPENDIX D — INTERFACE BREAKDOWN 
Quick Access Toolbar, Ribbon, Prompt, and User Input ...... 44 
Structure Browser, Catch Toolbar, and Status Bar .............. 45 
File tab ..................................................................................... 46 
Modeling, Structure, and Feature Tabs ................................ 47 
3D Geometry, Analysis, and View Tabs ................................. 48 
Applications Tab ..................................................................... 49 
 
 
GLOSSARY 
Glossary ......................................................................... 50-51 
QUICK REFERENCE GUIDE 
 ii 
 
 
HISTORICAL OVERVIEW 
Creo Elements/Direct Introduction 
HISTORICAL OVERVIEW 
 The lineage of Creo Elements/Direct 
(CED) introduced the concept of dynamic 
modeling to mechanical designers across 
the world. Starting with 
ME 30, CED has been 
providing continuous 
improvement and inno-
vation for over 27 years. 
ME 30 
 ME30 isn’t actual-
ly the originating soft-
ware behind CED. 
SolidDesigner is. Still, 
ME30 provided the seeds that eventually 
grew into SolidDesigner. 
 Originally developed in Germany, HP 
Precision Engineering / ME30 (HP PE/
ME30) was released in 1986 by Hewlett 
Packard MDD (Mechanical Design Divi-
sion) . The first versions were exclusive to 
the HP-UX operating system, but a Mi-
crosoft Windows compatible version was 
developed as popularity grew. 
ME30 was based on the Romulus ker-
nel and therefore had an inherent issue 
with freeform surfaces. 
SOLIDDESIGNER 
 HP licensed the ACIS kernel in 1989 
for the PE suite. Solid Designer was devel-
oped shortly afterwards with freeform capa-
bility. 
HP PE/SolidDesigner began in 
1994 as a product-modeling 
suite simultaneously supported 
with ME30, but HP transitioned 
their customers from ME30 to 
SolidDesigner through 1995. 
 
COCREATE ONESPACE 
 CoCreate Software Inc. adopted its 
name in 1996 when it became a subsidiary 
of HP rather than the Mechanical Design 
Division thereof. 
 By 1998, HP CoCreate Software solu-
tions were installed in more than 30 coun-
tries on more than 120,000 systems. A 
testament to the success of the software. 
 Cocreate then became its own inde-
pendent entity in 2000. Two years later, 
the product line changed names and 
CoCreate OneSpace Modeling made its 
début. 
 
 HBK Investments took-over CoCreate Software Inc. in 2006. 
PTC purchased CoCreate from them in 2007 for roughly $250M. 
Shortly afterwards, PTC released CoCreate Modeling 2008 as the 
last revision with the historic interface (rev 16). 
 It wasn't until rev 16.5 in late 2009 that we started to see changes toward a mutual-
istic relationship with Pro/Engineer (Pro/E). 16.5 introduced the save-as functionality for 
the GRANITE and ProductView formats and an integration with Mechanica. 
CREO ELEMENTS/DIRECT 
 Creo Elements/Direct (Rev 17) came out in 2010. This is where we get our first 
taste of the sweeping changes to come. Two new commands appeared; Pull and Stretch 
Face. New functionality showed PTC’s willingness to continue the product line; Import na-
tive Pro/E data, improved dimensioning, better PCB interaction, additional constraint recog-
nition in the 2D Copilot, and more for a total of 30 major changes. 
 
 Creo Elements/Direct (Rev 18) appeared in 2011 and was the first time we saw the 
new Fluid UI common to the Creo applications. We also see 28 more major changes intro-
duced including the new Stretch Edge command and numerous functionality improve-
ments like improved data exchange with CP, cross-part move and stretch, and the impres-
sive Face Part Modeling. 
 PTC released Creo Elements/Direct (Rev 18.1) in 2012 with 
19 more major changes . Improved selection and stretching, 2D 
geometry and 3D wire parts added to Annotations, edge change 
commands, and much more. 
 PTC proved its commitment to product improvement and en-
hancement in Creo Elements/Direct and will carry it well beyond the 
next generation of CAD tools. 
Forward looking information is subject to change without notice 
QUICK REFERENCE GUIDE 
 iii 
 DIRECT MODELING IN CREO 
Creo Elements/Direct Introduction 
PARAMETRIC AND DIRECT 
 There are at least two distinctively different design paradigms in the 3D CAD 
world; Parametric and Direct modeling. They sit on opposite sides of the modeling 
spectrum, but PTC brought them together in the new Creo product suite. Learning from 
Creo Elements/Direct, PTC created Creo Direct and the Flexible Modeling Extension for 
Creo Parametric. PTC continues to significantly invest in expanding direct modeling in 
Creo and making direct modeling its core CAD strategy. 
DIRECT MODELING SOLUTIONS 
 Developers spent years perfecting techniques to trade data amongst CAD applica-
tions. Translation, feature recognition, 3D from 2D generation, and more. Most of 
these fall short of providing what the parametric industry needed for years; a method to 
effectively manipulate foreign data without re-creation. 
 Direct modeling provides that and much more. You gain the ability to better ad-
dress late stage changes, generate faster concept designs, have an easier time with 
model simplification, and include more people in the design workflow. The cost is typi-
cally the loss of your design history. PTC eliminated that drawback with the interaction 
between Creo Parametric, FMX, and Creo Direct. Designers now gain the power of di-
rect modeling without giving-
up design constraints. 
FLEXIBLE MODELING EXTENSION 
 
 Flexible Modeling Extension (FMX) for Creo Parametric (CP) lends the paramet-
ric user the ability to manipulate existing parametric or neutral parts using di-
rect modeling techniques. The interface has been stylized after Creo Paramet-
ric for ease of use. The commands are deceptively simple and easy to pick-up. 
The move command itself has an incredible array of options to explore once you under-
stand the basic concepts. Each direct command creates a new feature on the history tree 
which adds a new dimension to parametric mod-
eling. You can not create new geometry with it, 
but you don’t need to. You can use CP’s full ca-
pability to create any new geometry seamlessly. 
CREO ELEMENTS/DIRECT 
 A portion of the technology from CoCreate now appears in PTCs new CAD suite of 
products under the CREO moniker. The original application has been re-named, re-faced, 
and re-distributed as Creo Elements/Direct, but is not actually part of the Creo suite. The 
term “Creo Elements” is meant to describe that the original application was one of the 
elements used to create the new Creo framework, but does not reside within the frame-
work itself. 
 Productview and Pro/Engineer were the other two technology platforms that formed 
the basis for Creo. They were re-named at the time as well to Creo Elements/View and 
Creo Elements/Pro respectively. Those applications, however, have new incarnations 
inside of the Creo framework. Creo View/MCAD and ECAD both replaced Productview. 
Creo Parametric replaced Pro/Engineer. Creo Elements/Direct continues as its own ap-
plication suite. 
 
CREO DIRECT 
 
 Creo Direct (CD) is a new stand-alone application within the Creo suite. Very simi-
lar to FMX in functionality, Creo Direct comes with the additional abilityto author 
new geometry using direct modeling techniques, but no 2D drawing capability. 
The interface leans more towards new users and further away from seasoned para-
metric ones. There’s a click-through workflow where one operation ends by starting another, 
and a mini toolbar that appears with feature options while you work. The intent is for some-
one without parametric modeling experience to 
participate in the design. One can then Round-Trip 
data between Creo Direct and Creo Parametric with-
out any need for translation while retaining all de-
sign history. 
 
 
NOTE: Creo Direct will continue to grow in features and may eventually replace the Creo 
Elements/Direct product line, but Creo Direct has a long way to go and PTC is committed to 
continuing support and enhancement for Creo Elmenets/Direct for many, many years. 
ALERT: Creo Direct is not a continuation of 
CoCreate inside Creo. It’s a re-birth. 
NOTE: FMX modifications become more difficult as 
the model’s shape becomes more organic. 
QUICK REFERENCE GUIDE 
 iv 
 CREO ELEMENTS/DIRECT NEW FEATURE HIGHLIGHTS 
Creo Elements/Direct Introduction 
MIDDLE CLICK BEHAVIOR 
 When the cursor is over a current 
viewport, you can middle-click to perform 
the following operations: 
 Middle-click to end a command 
 Middle-click and rotate (or 
press CTRL, middle-click, and 
drag the cursor) to zoom. 
 Middle-click and drag the 
cursor to rotate (spin). 
 Press CTRL and Shift, mid-
dle-click, and drag the cursor 
to rotate elements in the view-
port around a point. 
 Press SHIFT, middle-click, 
and drag the cursor to pan. 
 To change the mouse 
interaction mode, click File
SettingsViewport. The View-
port Settings dialogue box 
opens. Then click the CoCre-
ate mouse interaction mode 
check box in the Dynamic 
Viewing pane of the Viewport 
Settings dialog box. 
 
CREO ELEMENTS/DIRECT NEW FEATURE HIGHLIGHTS 
 PTC implemented many major enhancements to Creo Elements/Direct, roughly 82 since rev 16, and is committed to the continua-
tion of those improvements. Many of those changes had drastic impact on the modeling environment. Like Creo Data Exchange, Para-
metric Assemblies, Outline Views, Cross Part Move-and-Stretch, Enhanced 2D CoPilot, Projected Profiles, Modify Edges, and many more. 
Four of those improvements, though, stand out above the rest. Stretch Faces, Stretch Edge, Pull, and Face Part Modeling. 
STRETCH FACES 
 You can now move a 
face while maintaining their 
boundaries and adapting the 
neighbor faces. This new 
Stretch command strongly 
resembles the stretch feature 
in 2D where you move e.g. a 
straight line and the connect-
ed edges are adjusted like a 
rubber band. You can also 
stretch several unconnected 
faces at the same time. 
STRETCH EDGE 
 The new Stretch Edge 
command is the logical next 
step beyond the Stretch Face 
command. Stretch Edge al-
lows you to move edges (one 
per face), automatically ad-
justing the affected faces. 
Some model changes that 
required several steps before 
can now be performed in one 
operation. 
PULL 
 You now have one oper-
ation that combines the Ex-
trude, Mill, Turn, Bore, and 
Linear and Angular Lift com-
mands. The new Pull com-
mand simplifies the user inter-
action. When selecting a work-
plane, closed profile areas are 
automatically detected and 
highlighted as pre-selected. 
Pull can also work with select-
ed faces. 
FACE PART MODELING 
 Parts that do not repre-
sent a closed volume can be 
modified like solid models as 
long as the open boundaries 
are not affected. This situation 
often arises when imported 
models don’t match the receiv-
ing system’s accuracy require-
ments. Repairing such models 
requires expert skills which is 
not a good prerequisite for 
potentially simple changes. 
NOTE: You can also right-click the 
current viewport and drag to pan. 
NOTE: For the complete list of updates from Rev 16 to current, please visit: 
http://www.ptc.com/appserver/wcms/relnotes/?show=y&product=137115 
Or search on http://www.ptc.com/ for Enhancement Details. 
http://www.ptc.com/appserver/wcms/relnotes/?show=y&product=137115
http://www.ptc.com/
QUICK REFERENCE GUIDE 
 1 
 MODELING: BASIC MODELING 
Modeling 
INTERFACE SUMMARY 
 
 
 
 
 
 
 
 
 
 
 
 
 
Browser Bar The 
browser bar shows all 
opened browsers; for 
instance the structure 
browser. The struc-
ture browser displays 
all 3D objects and 
elements (parts, as-
semblies, workplanes, 
and so on) and their 
interrelationships. 
User Input Line Used to enter commands, general ex-
pressions, or text. On by default and can be shown us-
ing the Ribbon ViewToolbarsUser Input Line. 
Status Bar Shows the alert history, current work-
plane, part, and settings for Catch and Units. 
Also shows pre-selection focus, quick viewport 
settings, and a "previous application" switch. 
Configurable on right-click. 
Prompts By default, displayed in the status bar. Provides gen-
eral feedback, messages, and guidance. Can be added to a 
Prompt Bar using the Ribbon ViewToolbarsPrompt Bar. 
Quick Access Toolbar Provides quick access to frequently-used commands. You can 
customize it by adding, removing and reordering commands (buttons and groups) to it. 
Ribbon Contains commands organized as a 
set of tabs. On each tab, related commands 
are grouped. Fully customizable. 
Mini Toolbar Helps you to quickly execute a 
command from the viewport, and changes 
content based on current selected object and 
context. The first command is the default 
for that operation. Fully customizable. 
OK, Cancel, and Detail Buttons 
These buttons are only available 
if a command is active. Check 
mark to complete, ex to cancel, 
and triangle to view Command 
Details dialogue box. 
Command Details 
Opens by activating 
the Detail Button. 
You can select 
elements or set 
properties, com-
plete or cancel the 
command, and get 
quick access to help. 
Context Menu Opens when you select 
and right-click any element in the view-
port in the pre-selection mode. Depend-
ing on the current context and selected 
object, the commands change. 
File Tab Unique tab providing the application’s most intrinsic 
commands. Session and file operations, settings and options, 
module and application activation, command search, and exit. 
TIP: You can press SPACEBAR 
to open the Mini Toolbar and 
click on its to open the 
Command Details during an 
operation. 
QUICK REFERENCE GUIDE 
 2 
 MODELING: BASIC MODELING 
Modeling 
WORKING WITH FILES 
 Creo Elements/Direct is a session 
based software rather than file based. This 
allows it to open multiple files at the same 
time. Opening new files adds them to your 
current session. 
 When saving, you’re asked to provide 
what, where, and how. Select what objects, 
parts, and/or assemblies to save. Then 
direct the file browser to the desired save 
location. Finally, choose your preferred file 
format. 
CED interacts with a large array of file types. 
These are the native file types typically used: 
 
*.pkg — Package. Some or all of the 3D data for a 
 project in a single file. 
*.bdl — Bundle. Assembly and/or 3D model and 
 associated drawing stored together. 
*.sd* — Individual 3D Content and Instance data 
 files. 
*.ses — Session. All parts, assemblies, 
 workplanes, and settings like units, 
 lights, viewports, etc. 
*.env — Environment. All active environment 
 settings. 
*.mi — 2D drawings and annotations. 
WORKING WITH THE RIBBON 
 The ribbon UI provides an efficient layout for modeling commands. The most frequently used commands are displayed in large icons. 
Uncommonly used commands are grouped into submenus within each section of the ribbon The commonly used Utilities section is available 
in most tabs. Settings for each functional area are groupedwith the modeling functions. 
 
RIGHT-HAND RULE 
 The right-hand rule has been around 
for a long time, and is still commonly re-
ferred to today. It’s a mathematical mne-
monic for understanding 3 dimensional 
vectors. There are several ways to use the 
right-hand rule, but it’s generally referred to 
in association with rotation in CAD. 
 If you choose an edge as your rotation-
al axis, and a positive number for your rota-
tional value, will the subject turn inward or 
outward? Right or left? 
 
 If your rotational axis’s positive direc-
tion is your right thumb as it points in a 
“thumbs up” gesture, then a positive num-
ber will rotate your subject in the direction 
your fingers curl. 
TIP: Some object or file-type selections will 
only correspond to their respective file-types 
or objects. Don’t be surprised if your options 
change based on what you click. 
BEST PRACTICE: If you’re working directly 
with 3D files, and not using a data manage-
ment solution, use “Package” (*.pkg) as your 
go-to file format. Otherwise, packages are not 
recommended due to their file size and prob-
lems generated from a broken file stream 
when saving in a PDM or PLM environment. 
Common Un-Common 
Settings 
TIP: You can add commands to the Quick Ac-
cess Toolbar directly from your search results. 
MINI TOOLBARS 
The operations mini toolbar offers di-
rect access to commonly used operations 
based on your operation without having to 
traverse the ribbon. The most common 
command is automatically activated without 
having to be selected. The list of commands 
can be customized to suit your needs. 
 
 
The options mini toolbar offers addi-
tional options during an operation. To acti-
vate, press the SPACEBAR. This has the 
added benefit of bringing the operations 
toolbar back into view if it’s faded. 
Functional Areas Divided Into Tabs 
Closely Related Command Groups 
Operations Mini Toolbar 
Options Mini Toolbar 
COMMAND FINDER 
 Open the File Tab. At the bottom is a 
search window used for finding commands. 
The search assumes a wildcard on either 
end of your entry. It doesn’t search the 
command description, but will search the 
FULL command name; displayed or not. 
 
 
 
 
 
 
BEST PRACTICE: It is always preferable to 
work with a PDM or PLM rather than a file 
system when possible. 
QUICK REFERENCE GUIDE 
 3 
 MODELING: BASIC MODELING 
Modeling 
DIALOGUE BOXES 
Command dialogue boxes display your 
current option sets, but also typically require 
some additional information before being 
able to complete the command. To provide 
the required information, you can click an 
item in the viewport or structure browser if 
you need to choose a face, object, drag an 
angle, pull a position, etc. You can also type 
data in a yellow field if the information can 
be given alphanumerically. For example, for 
Model Name you can type “p1” to specify a 
part rather than selecting it in the viewport 
or Structure Browser. The forward slash 
prefix “/p1” isn’t required. Spaces are not 
allowed for parts, assemblies, or file names. 
TIP: If you use a postfix to specify measure-
ment units, they are converted to the sys-
tem’s current units. Math is also supported. 
 
Length Units: um, mm, cm, m, km 
 uin, mil, inch, foot, yard, mile 
Angle Units: deg, rad, grd 
Angle Convert: Degrees:Minutes:Seconds 
Math: 
RIGHT-CLICK DIALOGUE 
Right-clicking in a dialogue box that can 
accept numeric entries will provide a contex-
tual menu designed for your input options. 
It offers a list of the last values you’ve en-
tered into similar boxes, a link to measure-
ment based on the dialogue box type, a link 
to the calculator, and quick access to your 
copy/paste functionality. 
From the Calculator, you can use the X 
box to the left of your numerical entry win-
dow to send your product back to the dia-
logue box. 
From the measurement output dia-
logue, you can use the leftmost green arrow 
to send your measurement back to the dia-
logue box. If you need to do some calcula-
tions first, use the green arrow with the cal-
culator icon to send your measurement to 
the Calculator command. 
 
 
 
From the measurement dialogue you 
can select any of the different types of 
measurement if the one selected was not 
what you truly needed. 
ALERT: You can’t use unit conversion and 
math in the same step. 
= 
= 
= 
+, -, *, / 
sin, cos, tan 
asin, acos, atan 
sqrt (square root) 
exp (e^x) 
PI (or lower-case pi) 
bracket terms 
floor(n) (highest integer less 
 than or equal to n; 
 rounds n down to the 
 next integer) 
ceil(n) (smallest integer not less 
 than n; rounds n up to 
 the next integer) 
^ (power: x^y where Y is an 
 integer 
CALCULATOR 
The utilities 
command group 
is repeated in 
most tabs. In the 
lower right corner 
of the utilities 
group you’ll find 
the Calculator command. 
Change the calculator from a standard 
(the default) to a Reverse Polish Notation 
(RPN) calculator from File  Settings  
System. 
Use the EngLen, Dist, Rad, Ang, 3D, 
and Prop buttons for a variety of measure-
ment options. Use the measurements di-
rectly in your computations and copy/paste 
your solutions back to dialogue boxes or use 
the X button to send them to your active 
dialogue box. Use the scroll bar (circled in 
red on the lower right of the illustration) to 
see additional math operations. 
RPN CALCULATOR 
 
EXTENDED OPERATIONS 
 
 
 
 
 
 
R->P and P->R are exclusive to the RPN 
calculator. Also, y^x is x^y in the standard 
calculator. 
QUICK REFERENCE GUIDE 
 4 
 
INTRODUCING WORKPLANES 
 The workplane (WP) is a 3D represen-
tation of an infinitely large plane. This is 
where you define all 2D geometry for mod-
eling. It has its own coordinate system with 
a u, v, and w axis. You can have multiple 
workplanes defined, but only one can be 
active at any given time. 
Default Workplane: Most basic WP. 
Its origin is aligned with the global 
coordinate system upon creation. 
Workplane on Face: The most com-
monly used WP. Once you have a 
face selected, hold ALT and middle-
click for an instant WP. You can also grab a 
draw tool and simply start drawing on a 
face. The WP will be generated for you. 
Workplane on Axis: When working 
with a cylindrical part, a WP aligned 
with its axis is often needed. The 
new WP can align its u, v, or w axis 
to the part’s center axis by select-
ing a curved surface as reference. 
BEST PRACTICE: Workplanes can be deleted. 
Try to keep their number to a minimum. Or-
ganizing, categorizing, and managing the 
display of many used workplanes can unnec-
essarily clutter your design. 
TIP: It may be easier to line-up your axis WP with 
the Pt on WP option to anchor to a specific point. 
POSITIONING WORKPLANES 
Use the work-
plane positioning 
options to move your 
workplane to exactly 
where you need it to 
be. Use the mini toolbar or right-click while 
the workplane is selected in your 3D view-
port. Position the 
workplane using 
the 3D CoPilot 
and/or the meth-
ods available in 
the command 
dialogue box. 
You can 
change the work-
plane’s origin by 
using the Slide 
WP Origin com-
mand. It can be 
found in the 
Structure Tab in 
the Workplane 
group under the 
More menu. 
Click a point 
on the workplane 
or type the point 
position relative 
to the old workplane origin. 
CONSTRUCTION GEOMETRY 
Construction geometry is generated 
using many of the same 2D drawing 
methods as real geometry. It’s used to 
create references for real geometry 
creation, and can even be traced over 
with real geometry using the Overdraw com-
mand. You can also use it as a guideline 
for machine operations like turning 
an axis. 
REAL GEOMETRY 
 Real geometry is directly used 
for machine commands. Any remain-
ingconstruction geometry is ignored. 
 In addition to the typical line and 
circle creation commands, you can 
create a variety of rectangles, arcs, 
splines, and project 2D geometry from 
faces, edges, cross-sections, and out-
lines. Real geometry can be modified 
with fillet, move/stretch, trim, rotate, 
scale, mirror and more. 
Delete 2D geometry by selecting it and 
using your Delete key or right-click menu 
delete option. 
NOTE: The workplane UVW axis starts off in the 
lower left of the workplane. (as viewed from +W) 
When you reposition the origin, it does not retain 
this boundary relationship. From then on, the 
boundary is centered on the UVW where possible. 
The workplane grows off center to encompass all 
contained 2D geometry. 
CREATING 2D GEOMETRY 
Use the 2D Geometry creation tools 
under the Modeling tab in the Draw group. 
All 2D geometry is created on a workplane. 
In fact, you can only create, modify, or de-
lete geometry from the active workplane. 
Aside from your basic geometry, you 
can create arcs, splines, ellipses, functional 
and conical curves, fillets, and equidistant 
offsets. 
The Overdraw command 
is used to draw on top of con-
struction geometry to create 
real geometry. The usage of 
Overdraw depreciat-
ed with the advent of 
the 2D and 3D CoPi-
lots, but can still be 
very useful. 
Quickly swap 
between geometry 
and construction 
with the Overdraw dialogue box options. 
The tracking options allow you to choose 
what your traces snap to; real geometry or 
construction geometry. You can also decide 
to compute the intersection between your 
contour and edges. Uncheck to ignore inter-
sections for faster performance. 
If you take a wrong turn, use the Back 
button in the dialogue box to return to the 
previous selection. You can also click your 
last profile point or use the Z key to return to 
the previous selection. 
NOTE: You can also draw 2D geometry on Docuplanes 
from the 3D Documentation application. 
MODELING: BASIC MODELING 
Modeling 
QUICK REFERENCE GUIDE 
 5 
 MODELING: BASIC MODELING 
Modeling 
THE CATCH TOOL 
The Catch tool defines how your cursor 
catches or snaps to the elements defined 
in the 2D and 3D Copilot settings. It’s an 
integral part of the environment, and a core 
piece of the 2D drawing and 3D modeling 
experience in CED. As you mouse-over 
geometry, the catch tool gathers references 
based on those snap settings. For exam-
ple, if you mouse-over an edge, that edge 
will be referenced in your 2D sketch. To 
clear the reference memory, hit the Delete 
key. You can access the catch settings 
from the Catch label on the status bar. 
 
 
 Within the Catch settings you have a 
dropdown for Next Catch, Default 2D, and 
Default 3D. This dropdown indicates which 
group of Catch settings you’re affecting 
with your changes. 
Next Catch settings only apply to the 
very next caught entity — The one-off catch-
es needed as you sketch. It returns to de-
fault after the operation if it was changed. 
Default 2D and Default 3D refer to the 
default behavior in 2D mode and 3D mode 
for your next catch and every subsequent 
operation. Take care when making chang-
es to these settings. 
By default, Default 2D catches to all 
geometry elements on the active workplane 
and projects the point onto the workplane. 
By default, Default 3D catches all ge-
ometry elements on all workplanes and all 
parts. 
THE 2D COPILOT 
The 2D CoPilot can assist in creating 2D geometry without using construction geome-
try. It’s an interactive tool with automatic snaps, real time referencing and feedback, and 
relative measurement capability. Access the 2D CoPilot settings from the Draw and Modify 
2D command groups under the Modeling tab or File Settings 2D CoPilot. 
 Combining the catch tool and 2D CoPilot, the drawing 
experience is enhanced significantly. For example, in the im-
ages above, the 2D CoPilot guides the creation of the new line 
by indicating newline length, distance to horizontal reference, 
angle from existing geometry, parallelism and perpendicularity to existing 
geometry. In a typical workflow outside of CED, you’d need to create those 
references through the use of construction geometry in many cases. 
Further, you can type dimensional values where applicable by clicking the TAB key to 
cycle through available dimensions. You can also alter the snap-grid precision by using 
PgUp and PgDn. For example, dragging your line may progress from 14 to 15 and 16. Af-
ter pressing PgUp, the numbers jump from 10 to 20 and 30. Similarly, using PgDn can 
take the dimensions down to 2 decimal places while dragging. Home key resets. 
The little keyboard icon appears when you have a Mini Toolbar available. Use the 
SPACEBAR to open the Option Mini Toolbar or click the keyboard. Click the button 
for a list of available shortcuts. Access relative measurement, bends, the back command, 
ignore o r lock snaps, and more in a context sensitive list with shortcut hot-keys listed. 
Use the Set Length or Set Angle command to constrain your lines. Use Set Radius to 
constrain your circles, or swap between rectangle types using their respective commands. 
 
New Line 
Catch Points 
LOCKING CONSTRAINTS 
You can lock or unlock (by use of the L 
key) snapping conditions as they appear in 
the 2D CoPilot to restrict the movement of 
your profile element during creation. The 
individual snapping conditions additively 
restrict degrees of freedom in the element, 
refining its final placement. 
You can recognize lockable constraints 
by the red lock that appears next to them. 
Locked constraints 
will appear red them-
selves and must be 
unlocked in the same 
way to restore free-
dom of movement in 
that direction. 
Multiple locked con-
straints, while having 
a beneficial additive 
effect, can also be-
come too difficult to 
navigate as refer-
ence combinations 
bind movement con-
trary to the desired effect. You can unlock 
or explicitly ignore (by use of the I key) spe-
cific constraints or clear the buffer entirely 
with the Delete key. 
KEYBOARD INPUT 
Type 2D coordinates at any time to 
start or end a single line, rectangle, or speci-
fy the center of a circle. Entering a number 
during line creation indicates length. A sub-
sequent number will be its angle. Circular 
entities will have their radii defined. 
QUICK REFERENCE GUIDE 
 6 
 MODELING: BASIC MODELING 
Modeling 
MODIFY 2D 
The basic Modify 2D commands like 
Rotate, Move, Scale, Mirror, and Stretch will 
change the geometry by either location, size, 
or orientation. Convert Geo toggles geome-
try types between real and construction. 
Use the trim and extend commands to re-
pair 2D geometry. 
MOVE AND STRETCH 2D 
You can activate Move 
and Stretch from the com-
mand button, but get a wid-
er array of fast options from 
the Options Mini 
Toolbar by simply 
clicking on a piece 
of 2D geometry. 
 
TANGENCY 
At any point during line creation, use 
the Options Mini Toolbar to override any 
active snaps and use the Tangency snap. 
SET MIRROR 
Mirroring your 2D geometry real-time 
couldn't be simpler. Use your Options Mini 
Toolbar, select Set Mirror, and choose a 
mirror line/reference. 
RELATIVE MEASUREMENT 
Create any 2D geometry relative to 
existing geometry or references. Tap the R 
key to start a relative measurement. The 
point or line your cursor was over at the time 
is immediately used as a reference point. 
You can use multiple references for a single 
command. For example: 
Start a new rectangle and catch a verti-
cal reference. Then tap R to define that 
vertical reference edge as a relative meas-
urement reference. 
Then move to a horizontal reference, 
and tap R again. 
 
 
 
Notice that the 2D CoPilot is already 
using the first reference for a relativedi-
mension. Now that you have both refer-
ences, you can either type manual dimen-
sions (cycling with Tab) or drag your refer-
ences out to the desired starting point and 
left click to begin your rectangle. 
PUTTING IT ALL TOGETHER 
Mastering 2D drawing in Creo Ele-
ments/Direct will require using all of these 
features together. Particularly, get use to 
using your hot-key commands. 
 
 R for relative measurement. 
 B to create a bend (arc). 
 Z to undo your last 2D command. 
 SHIFT pressed to suspend snapping. 
 I to ignore a snap. 
 L to lock/unlock a snap. 
 Delete clear Catch memory. 
 SPACE for your Mini Toolbar. 
 PgUp increase adaptive grid size. 
 PgDn decrease adaptive grid size. 
 Home reset adaptive grid size. 
 Shift+Ctrl to snap to a center. 
Relative measurement can be used mid
-sketch. Not just to initiate a sketch. Any-
time you want to place a point relative to 
another location, use R. 
Using B to create an arc can save you 
from creating construction circles and arcs 
with Overdraw to get what you need. Press-
ing B when your cursor is positioned as a 
continuation of the previous line will start 
arc tangent to the previous line. Pressing B 
when your cursor is positioned at an angle 
to the previous line will start an arc that’s 
tangent to that angle. 
Easily recover from missteps with Z. 
New users will tend to finish the 2D com-
mand, delete unwanted geometry, then 
begin again. Some will delete the workplane 
entirely and start fresh. This interrupts the 
rhythm of your design process and con-
sumes valuable time. Get familiar with us-
ing Z to simply back-up one step. 
Snaps can be extremely valuable while 
drawing in 2D. Using I to ignore some snap 
conditions may open-up further snaps that 
you may have been looking for but were 
considered lower priority. Use SHIFT, I, and 
L to traverse snap conditions quickly. Use 
Delete to wipe your current snap conditions 
and start over. 
Change your snap options to suit your 
needs under your 2D CoPilot settings. 
Orange symbols appear when the snap 
is activated against existing geometry. The 
adjoining geometry will also be highlighted 
in orange. If the snap represents a theoreti-
cal relationship provided by the 2D CoPilot, 
the icon will be in cyan. These symbols 
gives you the opportunity to suppress, ig-
nore, lock, or just run with the snap. 
 
 
TIP: You can use H to show/hide the 2D CoPilot cursor 
text that normally shows u,v position or dimension text 
TIP: In Creo Elements/Direct Trim, you pick what you 
want to keep. Not what you want to delete. 
Perpendicular 
Vertical 
Horizontal 
Tangent 
Parallel 
QUICK REFERENCE GUIDE 
 7 
 MODELING: BASIC MODELING 
Modeling 
REFERENCE CONES 
The green and red reference cones act 
as anchors for the dimensional definition of a 
3D modification. For example, if you were to 
pull a face, the default anchors would give 
you a dimensional reference that indicates 
the from-to change. What if that wasn’t your 
aim? Maybe you were interested in the re-
sulting overall length of the part after the 
modification. 
Traditionally, you’d need to measure the part, 
subtract its current length from the desired 
length, and then enter the remaining amount 
in your modification. In this case, though, you 
only need to click the red anchor, click the 
rear of the part, and type-in or drag to your 
desired dimension. 
3D COPILOT 
The 3D CoPilot ap-
pears in many forms de-
pending on the context of 
your modification. In every 
case, though, its job is to help 
you clarify a 3D set of con-
straints in a clear and easy 
manner. 
The blue widget is looking 
to be placed on an appro-
priate reference. The or-
ange widget (in whole or in 
part) is anchored to your 
reference and displays your 
degrees of freedom. Select 
an axis for linear move-
ment, a toroid for angular, 
or one of the planes for 
planar movement options. 
The green reference dia-
mond indicates that you 
can change the origin of 
the 3D CoPilot widget. 
The red reference dia-
mond indicates an origin 
change. You’ve selected 
a green reference dia-
mond, and now need to use 
the new widget to re-position 
the 3D CoPilot widget. When 
you’re done, select the red 
reference diamond to com-
plete the movement. 
Change the settings from File Settings 
3D Copilot. 
NOTE: Operating the 3D CoPilot is a click and re-
lease interface. There is no drag-and-drop. 
SELECTING REGIONS 
A 2D profile must contain at least one 
closed loop, but that’s the only restriction. 
You can have several loops, extraneous 
geometry, and construction lines. Once 
you’re done with your 2D profile drawing, 
middle-click or click the check mark to 
complete. When you Pull the profile (or 
another command, but Pull is most com-
mon), you’ll be given the opportunity to 
select which closed loop (region) you wish 
to use for the given command. 
Simply click on the closed loops until 
you have the desired region(s) selected. 
 
UNDO AND REDO 
On the Quick Access Toolbar, you can 
undo or redo one step at a time. You can 
also click the down arrow next to the undo/
redo icons to select the number of steps 
you want. If you want to view the history 
before making your choice, click Expand. 
Creo Elements/Direct tracks both the 
command history and the history of any 
active module applications. When you un-
do, you may get a warning that you’re about 
to undo a module application 
command. 
TIP: If you click on the workplane border to 
start a Pull, as shown here, you can immedi-
ately start selecting regions and continue the 
pull by then clicking on the 3D CoPilot widget. 
If you instead execute the Pull command from 
the ribbon or mini toolbar first, you’ll need to 
open the dialogue box and change the Select-
ed option to modify the selected region(s). 
QUICK REFERENCE GUIDE 
 8 
 MODELING: BASIC MODELING 
Modeling 
THE PULL COMMAND 
Extrude, Mill, Turn, and Bore have been replaced by Pull. The Pull command actually con-
tains a combination of two 2D profile commands (Linear Pull Profile and Angular Pull Profile) 
and two 3D modification commands (Linear Pull Faces and Angular Pull Faces). 3D modifica-
tion is covered elsewhere in this guide. 
Linear Pull Profile and Angular Pull Profile are the main focus for most 3D geometry crea-
tion from 2D profiles. You can activate the Pull command by clicking on the command ribbon, 
left-click on your workplane border, or double left-click on the 
workplane representation in your structure browser. The only 
difference being that the command ribbon option automati-
cally assumes all closed loops in your profile are to be pulled. 
If you intend to change the region selections, you’ll need to 
modify the selection list through the command dialogue box. 
The default command is Linear Pull Profile when using 
pull on a 2D profile. To change this option to angular pull, 
use the Option Mini Toolbar or change the command dia-
logue box. 
The Linear Pull Profile will provide a linear 3D CoPilot 
widget for the pull along with Reference Cones to refine the 
distance after the initial definition. 
The Angular Pull Profile will provide a reference 3D CoPi-
lot widget for you to place on an edge, axis, line, or oth-
er axial reference (see Right-Hand Rule). Then, a rota-
tional 3D CoPilot widget appears to define the angle of 
the pull. 
Add/Remove Material. Each of these commands 
will attempt to automatically add or remove material 
from your existing part (if one exists). Sometimes, the 
automatic determination is not what you want. You can 
change this option in the dialogue box under Method  
Operation. 
3D Snapping. Your Pull Profile can terminate with a fixed 
dimension or a reference to an existing element. 
 
 
You can change which 
elements aresnapped to un-
der the Type option for the 
command. It can be changed 
to Part, Face, Point, or Plane. 
Change Direction by dragging your 3D CoPilot widget from 
one side of the starting workplane to the other or use the Direc-
tion option in the command 
dialogue box. The dialogue 
box has the added capabilities 
to extend your profile from 
both sides of the workplane or 
take a User Defined approach 
to the pull direction. 
Specify a Draft Angle between 90 and –90 degrees. The 
draft works much like a Taper Face command using the work-
plane as your draft plane and the entirety of your profile to deter-
mine the faces to be changed. 
TIP: The 3D CoPilot attempts to snap 3D references you mouse over. 
ALERT: To intersect a part, the profile must be fully bound inside the 
intersecting part. You can overlap with face, point, or plane, but not part. 
QUICK REFERENCE GUIDE 
 9 
 MODELING: BASIC MODELING 
Modeling 
SELECTION 
Before you can dynamically modify 
geometry, you need to select it. Creo Ele-
ments/Direct provides everything you need 
to make selections on-the-fly. 
Click Selection: This is the most intui-
tive and simplistic selection method. Driven 
by mouse-over, the click-what-you-want 
method is your first tool. Simply mouse-over 
what you want until it highlights, then left-
click. If you need more, shift-left-click to 
start a Selection List instead. 
Tab Selection: This is a geometry 
based selection method. This huge time 
saver grabs geometry by applying rules to 
the mouse-over target. Mouse-over a face 
until it highlights. Then press Tab. The Tab 
Selection method will grab all faces possibly 
associated with your mouse-over target by 
rule definition. To switch rule definitions, 
press Tab and your selection will change. 
Cycle through with Tab until you have what 
you need and then left-click to complete the 
selection. If you need more, shift-left-click to 
start a Selection List instead. 
Select Mini Toolbar: The Select Mini 
Toolbar isn’t a selection method in itself, but 
does provide access to three other selection 
methods. The toolbar is context sensitive. It 
will only appear when a selection method 
may be needed. Press SPACEBAR for the 
Mini Toolbar. 
 
 
 
The Geometry Rules allow you to create 
a custom rule configuration (like using Tab 
Selection) for selection criteria. 
Window Selection: Drag a window with 
a left mouse button held down. There are 
two possible results. First, everything within 
the window is selected. Second, everything 
within the window and everything intersect-
ing the window is selected. To toggle be-
tween the two results, hit Tab before releas-
ing the left mouse button. 
Selection List: A selection list is exactly 
what it sounds like; a list of multiple selec-
tions. You can start one multiple ways; shift-
left-click, select mini toolbar, through the 
Probe Selection dialogue, and through the 
Selection Tool. To add members to the list, 
select them using your preferred method(s) 
in any combination. To remove them, select 
them again. To end a list, middle-click. You 
can also end one from inside the Select Tool 
by clicking the List End button. 
Probe Selection: The probe selection 
tool allows you to select through a stack of 
elements piled on top of each other. To 
activate, use the Select Mini Toolbar, 
Ctrl+Tab, or the command icon Utilities sub-
group in the Ribbon UI. Once it’s been se-
lected, you can move your mouse around 
freely. Probe select will remember where 
your mouse was originally as the defining 
point for your probe selection. 
Selection Tool: The Selection Tool can 
be activated through the Select Mini 
Toolbar, in the Ribbon UI under the Utilities 
sub-group, or by pressing F2. It is the most 
powerful of your selection options, allowing 
for very precise selection criteria. 
The Selection Tool changes options 
based on its mode. Creo Elements/Direct 
chooses the mode for you based on the 
context of your operation. The modes are 
2D, 3D Elem, Feature, 3D Obj, and 3D Anno-
tation. 
The List menu provides a quick way to 
create a selection list of elements. This list 
interface has much more precise controls 
that are accessible by clicking the down 
arrows on the right of the List menu title. 
You get the new options Add, And, Remove, 
and XOR. 
XOR is the default behavior of selection 
lists. Click on an element. If it’s already 
selected, it’s removed from the list. If it’s 
not selected, it’s then added to the list. 
Add will do just that. Add the next se-
lection to your list. If it’s already a member 
of the list, it does not get removed. 
Remove is the opposite. Clicking on a 
list member will remove it from the list. 
Clicking on a non-list member will not add it 
to the list. 
And empowers the next selection to re-
form the list to include only members that 
were already in the list AND are in the next 
selection. Everything that doesn’t fit those 
criteria is removed from the list. 
The Elements area provides a radio 
button list of the valid element types you 
can select in the current mode. Choosing 
one will narrow your selections to those 
element types only. Initially, the most com-
mon elements are visible. Clicking the ar-
row button will expand the menu to include 
all possible options. 
The Boxing options are a representa-
tion of the Window Selection options for 
element intersection. 
The Methods options provide further 
refinement of your selection criteria. 
Choose a method to narrow your selection 
to related elements. 
Selection Tool 
Probe Selection 
Geometry Rules 
BEST PRACTICE: The combination of Tab 
Selection and on-the-fly Selection Lists is the 
fastest way to select subsets of complex ge-
ometry and will quickly become your most 
used selection method. 
QUICK REFERENCE GUIDE 
 10 
 MODELING: BASIC MODELING 
Modeling 
BLENDING 
Blends are generated on edges based 
on the neighboring faces and geometry. The 
edge where two faces meet is smoothed or 
blended by a singular or various radii. Creo 
Elements/Direct uses a rolling ball computa-
tion to generate these blends. 
 In the 
blend operation, 
only one blend 
face is created. 
If your geometry 
would require 
more faces to 
be generated to 
make your 
blend valid, Creo Elements/Direct will fail 
the blend operation. The model would re-
quire additional preparation before a proper 
blend could be applied. 
 You can create Constant Radius 
Blends, Var 2 Radius Blends, and Var N 
Radius Blends. “Var” refers to the bend 
radius as a variable number. In Var 2 Radi-
us Blends you specify the starting and end-
ing radii. In Var N, any number of radii at 
any location along the edge can be speci-
fied. 
 To create a blend, select and edge and 
choose your options from the mini toolbar, 
or click the command button in the Engi-
neering group of the Ribbon UI. 
Blends have four options for how they 
behave in relation to each other and exist-
ing geometry. 
Intersect is the default behavior and 
will ignore neighboring 
geometry. If the blend 
doesn’t fit, OnTanFaces is 
attempted. If both options 
fail, you’ll get an error 
message. 
OnTanFaces is the 
default fallback behavior. 
With it, a patch surface is 
created to get tangency of 
all faces. 
OnSharpEdge is really a variation of 
OnTanFaces. It adds the 
contingency of the blend 
running-in to a sharp edge 
(green). It will handle tan-
gencies in the same way 
as OnTanFaces (red). 
OnAnyEdge creates a 
sharp edge and surface 
patch to achieve its own 
tangency regardless of the 
neighboring edge type. 
CHAMFERS 
Chamfers behave similarly to Blends 
and are restricted by the same rules. You 
can create Distance, Dist/Dist, and Dist/
Angle Chamfers after selecting your edge or 
usingthe command button under the Engi-
neering group of the Ribbon UI. 
Distance Chamfers as-
sume a 45 deg angle and 
measures distance from the 
original edge to either of the 
two resulting edges. 
Dist/Dist chamfers only 
require two distances. The 
distance from the original 
edge to each of the two re-
sulting edges provided as 
two separate measurements. 
Dist/Ang chamfers 
need only one distance di-
mension and one angular 
dimension. You can swap 
which end of the chamfer 
you’re measuring for the distance dimen-
sion. 
RECOGNITION 
Recognizing blends and chamfers can 
convert them from extruded entities. This 
process will alter the behavior so that future 
updates will have the expected effect. 
Extruded cylinders will maintain a fixed 
axis. Therefore, when you change the radius 
of an extruded cylinder, neighboring faces 
will not maintain tangency. You’re left with 
a failed modification or a non-tangent round. 
When a typical blend is modified it al-
ways maintains the tangency with neighbor-
ing faces. To recognize blends, choose the 
command option under the engineering 
group and select the face(s) or part in ques-
tion. 
In a similar manner, geometry resem-
bling a chamfer can be just as important to 
recognize. A chamfer will reference the 
original edge when being modified. You can 
get away with modifying a chamfer using a 
move command if you don’t intend to 
change the angle, but even so, you wouldn’t 
have the same control over the chamfer as 
if it were recognized. 
BEST PRACTICE: It can be difficult to backtrack 
to your base geometry after adding complex 
cosmetic blends. Try to adding cosmetic blends 
at the end of the design. It’s best to meet your 
prismatic design requirements first. Some de-
sign houses will make a copy of the part before 
adding blends so that subsequent changes can 
be made from the base geometry. Blends start 
from scratch each time with that method, though. 
QUICK REFERENCE GUIDE 
 11 
 MODELING: BASIC MODELING 
Modeling 
MOVING FACES 
Moving faces looks a lot like a 2D stretch command in the 3D world. Select a face and 
the default command is Move 3D. It results in a 3D CoPilot widget and reference cones. 
The Move 3D can add or remove material and will attempt to do so 
automatically. You can change these options in the command dia-
logue. 
 You can use the same command to move multiple faces, assum-
ing the geometry lends itself to being altered in the desired direction. 
You can also grab multiple internal faces for modification. These are 
usually pockets of geometry that need to be resized or positioned. 
 In this case, you’ll likely want to change the origin for the move. 
Once you’ve selected the geometry and chosen the move command, click on an alternate 
face or edge to guide the movement. In the same way, you can make decisions about the 
kind of modification you want to make. If you change the origin of the move to an edge, you 
can either move the face(s) linearly along an axis or create a 
rotational movement (See Right-Hand Rule). 
Rotational movement can look like bending the model. 
When the face(s) is moved, the neighboring faces grow until 
they meet the modified face or other faces. 
The 3D CoPilot offers an easy and intuitive way to manage the move command. Individ-
ual dimensions can be typed, dragged, or snapped to geometry. 
PULL FACES 
At first glance, pulling faces may seem a lot like moving faces. Understanding the dif-
ferences can have a huge impact on your design. The Move 3D command will only grow 
neighboring faces. The pull command always adds faces unless new faces collapse into 
original faces. This offers flexibility to add design features without having to consider 
neighboring faces. 
The Pull 3D commands are option vari-
ants of the Pull command; Linear Pull Fac-
es and Angular Pull Faces (See Right-Hand 
Rule). 
 To activate them, either grab the command from the Modify 3D sub-
group of the Ribbon UI in the Modeling tab, or use the mini toolbar once 
you’ve selected your face(s). Use the 
command dialogue box to switch be-
tween the two commands without ending 
the operation. 
TIP: Hold down SHIFT during a Move 3D or Pull operation to snap to 
existing geometry courtesy of the 3D CoPilot. You can change this 
behavior to be automatic (not requiring the SHIFT to be pressed) by 
altering the 3D CoPilot snap settings. File Settings 3D Copilot. 
QUICK REFERENCE GUIDE 
 12 
 MODELING: BASIC MODELING 
Modeling 
STRETCH FACE 
 Immediately upon se-
lecting a face, the default 
command will be Move 3D. 
You’ll be presented with a 3D 
CoPilot widget and a Mini 
Toolbar to confirm the com-
mand. Right next to the Move 3D command 
is Stretch. 
The main difference between the two 
commands is that the Move 3D command 
grows neighboring faces while the Stretch 
command alters neighboring faces. 
In the conic illustration below, Move 3D 
continues the conic shape while Stretch 
translates the original face and stretches 
the neighboring faces to keep-up. 
Stretch Face has a much more dra-
matic impact when considering 3D altera-
tions that the Move 3D command has no 
comparison for. For example, in a cubic 
example, if you grab any face for Move 3D, 
your options are to extend the face in a 
positive or negative direction, adding or 
removing material as you go. The 3D CoPi-
lot widget seems to imply that you have the 
option to move in a parallel planar direct by 
way of the circular face presented on the 
widget. However, if you click the circular 
face, the Move 3D command can offer you 
nothing in that direction in most cases. 
If you’re using Stretch Face, 
though, you can turn a cube into a rhom-
boid, skew a cone, etc. 
Along the same lines, while rotating a 
face with Move 3D can have devastating 
effect depending on the 3D origin you 
choose, using Stretch Face for rotation can 
provide equally as devastating changes 
from the original origin. Once you start 
moving the origin around for Stretch Face, 
you can get all kinds of effects never before 
possible so quickly. 
STRETCH EDGE 
 Stretch Edge is the 
natural extension of Stretch 
Face. It allows the same 
power of Stretch Face, but 
with the precision of edge 
selection. The selected 
edge translates position while neighboring 
faces and edges stretch. 
CHANGE RADIUS/DIAMETER 
 When you 
take what we 
learned from 
Stretch Face 
and Stretch Edge and apply that to the 
Change Radius and Change Diameter com-
mands, you get an option to select an edge 
as opposed to being restricted to faces. For 
example, before you were able to grab a 
cylinder and change its radius/diameter. 
Now, you can select each end of the cylinder 
and modify the radius/diameter individually 
rather than needing to create a Loft or com-
plex revolve for the same effect. 
OFFSET FACE 
At first glance, Offset Face looks like a 
Move 3D command as used on any face. 
The power really shines when you’re offset-
ting groups of faces rather than a single 
face. While Move 3D will grab all the faces 
and translate them in the one direction you 
specify, Offset Face will move each face in 
the direction normal to each of the original 
faces in the selection group. It’s a great way 
to add/remove material on full or partial 
surface chains. 
On internal features, Offset Face can 
grow/shrink while Move 3D can only trans-
late. You’d need to Move 3D each face indi-
vidually to get a similar effect to what Offset 
Face can do in one operation. 
ALERT: While the Move 3D command is nearly 
a “no-fail” operation, Stretching Faces can pro-
duce bounding faces that cannot be enclosed 
in one volume. This will fail the operation. 
3D CoPilot Circular Face 
ALERT: Resulting surfaces have the potential 
to be undefined. This will fail the operation.QUICK REFERENCE GUIDE 
 13 
 MODELING: BASIC MODELING 
Modeling 
TAPER FACE 
 Taper Face is typically 
used to add draft to the mod-
el. To execute a taper, you’ll 
need a target face or faces, a 
draft plane, and a draft angle 
chosen in that order. Alternately, you can 
pick and choose the creation order through 
the command details dialogue. 
Change face. The target face(s) that 
will be altered by the operation. 
 Draft plane. This plane is meant to 
intersect with your change face(s). The line 
formed by that intersection creates the axis 
of rotation for each face. 
 You can select any 
planar entity as your 
draft plane or create one 
on the fly several ways. 
In the images, the draft 
plane is represented by 
a blue disc and axis 
widget. See how chang-
ing the draft plane dras-
tically affects the taper 
of the same four faces.
 Draft angle. The 
angle to be applied to 
the change against the 
normal of the draft 
plane along the inter-
secting axis. You can 
set the angle by using 
the 3D CoPilot or by 
typing a numeric value. 
Advanced Taper. With the standard 
taper you can only taper planes, cones and 
cylinders. The main difference is that, in an 
Advanced Taper, the resulting taper may not 
keep its original curvature. The face might 
be transformed into a freeform surface to 
satisfy your taper requirements. For exam-
ple, you might use an Advanced Taper for a 
rib that’s curved in the shape of an S. 
You can clearly 
see in the illustration that the curve on the 
top of the taper is completely different than 
the curve at the bottom, but the angle of the 
taper has been preserved. 
CUT, COPY, AND PASTE FACES 
A solid model is comprised of a series of connected faces. When faces are cut, neigh-
boring faces grow. Therefore, the result from cutting can be a removed feature, the model 
size may change, or the model is simplified. In a similar 
fashion, faces can be copied and pasted within the same 
part or between different parts. 
 Copy and pasting faces is 
one of the best methods for de-
sign reuse available in the envi-
ronment. To begin with, when you 
copy a set of faces you’re left with 
a Face Part. This face part is, by default, characterized as a cyan (light-blue) set of faces that 
are typically not solid on their own. The copy is completely independent from the original. 
When you paste the faces onto the same or separate part, you have the options to add or 
subtract the geometry from the paste target. Upon pasting, the faces can grow or extend 
themselves to match-up with the target area even if they previously did not touch. 
Notice that the subtraction worked like a cookie-cutter 
or ice-cream scoop. The direction of the subtraction is 
defined by the normal of the face part. To flip the normal, 
go to the Ribbon 3D Geometry 3D Surface Tools 
More Flip Faces. Alternately, you may want to solidify 
the face part first, then do a Boolean subtraction between 
solid parts. 
 
NOTE: The draft plane does not need to intersect 
the change face(s) visibly. The intersection can 
be theoretical as long as 
the planes intersect. 
Cut Faces 
Copy Faces 
Paste Add 
Paste Subtract 
TIP: When copying and pasting be-
tween parts, make sure that the parts 
are set to the same resolution first. 
Part Properties Geo Resol 
Resolution. 
TIP: Blends can be preserved in Advanced 
Tapers. The blends get removed, the taper 
is executed, then the blends get replaced. 
This is why you can’t specify the edge of a 
blend as a fixed edge in a taper. 
QUICK REFERENCE GUIDE 
 14 
 MODELING: BASIC MODELING 
Modeling 
PUNCH AND STAMP 
An easy way to remove material is by using the Punch tool to blast entire-
ly through a part in both directions. In fact, you can use Punch to go through 
an assembly as well. The same can be done with Pull, but by using Punch, 
you save yourself the trouble of dragging the 3D CoPilot entirely through the 
part/assembly. 
If you want to do the opposite of a Punch, where the 2D profile defines 
the geometry that remains instead of removed, you can use the Stamp com-
mand. Again, this could be done with Pull, but you’d need to draw a larger 
rectangle around your entire profile and part/assembly, then drag through. 
SHELL PART 
You can find Shell Part 
under the Modeling tab in the 
Model group. It removes mate-
rial from inside a part by remov-
ing one or more 
faces and add-
ing thickness to 
the remaining 
faces either 
inside or out-
side the original part. 
Turn a cylinder into a tube or cup, a 
cube into a box, or more commonly, shell a 
complex shape to create the beginnings of a 
plastic molded version of your design. 
 
SHELL FACES 
You can find Shell Faces 
under the Modeling tab in the 
Model group inside the Shell 
drop-down. While seemingly 
obscure, the Shell Faces com-
mand is another huge time 
saver. 
This command works 
similarly to Shell, but allows 
you to operate on parts that 
have already been shelled. 
Instead of requiring a full part, this al-
lows you to shell faces (or recognized fea-
tures) by any distance. You can update an 
already shelled part by first adding your 
feature and then using Shell Faces to shell 
the faces of the newly added feature. 
IMPRINT 
This command is used 
to create edges on a target 
part. Those edges can then 
be used to for separate 
operations themselves 
since they’re defining new 
face boundaries in your 
part. The commands can be found in the 
Modeling tab in the Model group. 
Linear. Use a sketch with closed re-
gions to define a new set of faces on your 
part. Linear will project your sketch from 
your workplane onto your part. 
Line does not have a dialogue box. It 
will ask you for a face and two points along 
edges over and over until you complete the 
command. It simply creates and edge be-
tween the two points along a face. 
Intersection will ask for a blank and a 
tool. The command will drawn an edge 
along your blank wherever the tool inter-
sects it. You also have the option of keeping 
the tool after the operation (default) or auto-
matically deleting it when the operation is 
complete. 
Silhouette is particularly useful for 
rounded and freeform surfaces. If you view 
a cylinder from the side, it looks like a rec-
tangle. View a sphere and it looks like a 
circle. That 2D silhouette is imprinted onto 
the object itself exactly along the viewed 
edge. Imagine tracing your hand as it lays 
flat on a piece of paper. This can alleviate 
the need to go through some complex work-
plane positioning gymnastics when you need 
to work with freeform surfaces. 
SECTION 
The Section command can be found along side Punch and Stamp under 
the Modeling tab in the Model Group and Remove drop-down. It’s not (by 
default) seen on the mini toolbar from a Pull command like they are, though. 
Section will divide a single part into one or more individual parts. It 
doesn’t remove any material, but does create new parts. To complete this operation you’ll 
need a part to be divided and some sort of tool or surface to execute the division. That enti-
ty can be a face or faces, a surface, plane, workplane and closed profile, another part, or a 
face part. 
A workplane with a profile will project the profile against the part (potentially in both 
directions off the workplane) and slice through as if the profile were a laser path. A face, 
part, surface, or face part must be in such a position as to completely divide your part exact-
ly where you want it divided. The new parts will perfectly conform to your dividing entity at 
the point of intersection. 
ALERT: Section is often confused with the Clipping Plane commands. Section will physically divide 
your part into separate pieces. It is not a visualization tool like Clipping Planes. 
QUICK REFERENCE GUIDE15 
 MODELING: BASIC MODELING 
Modeling 
BOOLEAN OPERATIONS 
Boolean operations are found on your Modeling tab under 
the Model group. Boolean refers to a logical combinatorial sys-
tem as implied by the logical operators of AND, OR, and NOT; 
adding, replacing, or removing material based on two or more 
entities. Unite, Subtract, and Intersect can use solid parts or 
face parts. The result will either be a solid part a face part 
based on the resulting geometry. 
Unite. Add material. This works somewhat like the Paste 
Face command except that parts will not be grown or stretched 
to meet each other like in 
the Past Face command. 
Two parts become one part. 
Any overlap or intersection 
between the blank and tool 
is combined into the result. 
Subtract. Remove ma-
terial. This command allows 
you use one part (or many 
parts) as the blank and one 
(or many) as the tool to cut 
away from the blank. Much 
like sculpting something out 
of clay, the Subtract command allows you to use a custom tool to cut away from existing 
geometry. You always have the option of keeping the tool in case you want to use it again to 
subtract in another location. 
Intersect. Replace ma-
terial. Intersect can use 
several parts as the blank and several parts for the tool. The resulting geometry will be a 
representation of only the intersection between the blank and the tool. Everything else is 
removed. 
Reflect. Is a special 
command. It’s a combina-
tion of Copy, Mirror, and Unite. Choose a part and a define a reflection plane. The part will 
be copied, mirrored about the reflection plane, and united with the original. You can choose 
to reflect material on one or both sides. Depending on the position of the reflection plane, 
Reflect can add, remove, or add and remove material. 
MIRROR PART 
Mirror can be found in the 
Modeling tab in the Modify 3D 
group in the More dropdown. It 
works differently than Reflect 
in that you’re mirroring an entire part(s) 
about the defined plane. Not mirroring ge-
ometry within a part. If you choose to keep 
the original, Mirror will create a new part in 
the mirrored position rather than mirroring 
the original. You can also mirror entire as-
semblies, workplanes, docuplanes, and 
layouts in this way. 
SCALE PART 
Scale can be found in the 
same dropdown as Mirror. You 
can change the size of parts 
are assemblies isotropically or 
anistropically. 
Isotropic scaling will change the tar-
get’s volume and its position relative to the 
global coordinate origin. A value larger 
than 1 will increase while values larger 
than 0 and smaller than 1 will decrease. 
Anistropic scaling approximates the 
shrinkage of molded plastic parts as they 
cool. You can specify scaling factors in the 
xyz directions to compensate for shrinkage. 
Scale the part or face by using values from 
0 to 1. For example, 0.9 would scale the 
part or face by 10%. 
ALIGN FACES 
Align can be found in the 
Modeling tab under the Modify 
3D group. It’s most commonly 
used to adjust faces such that 
they are aligned with another reference face
(s). For example, if you had 4 embossments 
of various heights and wanted to make sure 
that the tops were all on the same plane. 
You could manually adjust each, or you 
could select 3 of them and align to the 
fourth. There’s even an offset option if you 
wanted to select all 4 tops and offset them 
all from the base part in one command. 
A more advanced usage is to modify 
face topology to match an existing reference 
rather than re-creating. 
 
MERGE 
During the modeling pro-
cess, you can sometimes end 
up with situations where one 
part has overlapping faces or 
un-needed edges. Merge will 
combine faces by removing overlapping 
edges or combine edges by removing verti-
ces. 
Using Imprint can, in particular, leave 
stray edges on faces that should be Merged 
in the final design. 
 
ALERT: Use the Use Glue option only when the faces of the two 
parts match exactly and will not create an intersection of geom-
etry. Otherwise, the resulting part may become corrupted. 
ALERT: Never use identical parts in the same position for a 
subtraction. Use the Delete 3D function or right-click delete in 
those cases where a total removal is required. 
TIP: Try using Intersect for quick interference checking. 
TIP: If you have commonly subtracted geometry, try saving the 
tool off on its own. You can then reference it for future subtrac-
tions rather than re-creating it each time. 
BEST PRACTICE: Use Reflect to create symmetric parts. Create 
one half or quarter, then reflect them to complete your design. 
NOTE: Mirror can also be found in the Struc-
ture tab inside the Part & Assembly group. 
TIP: Try using Mirror for left-hand and right-
hand type part situations. 
QUICK REFERENCE GUIDE 
 16 
 MODELING: ADVANCED MODELING 
Modeling 
FREEFORM MODELING 
The name Freeform Modeling is really referring to the kinds of 
surfaces that can be created by the operations in this command 
group. Generally, freeform is used to describe surfaces that can’t 
be defined as prismatic objects like a plane or cylinder. In that 
way, you could group most of Creo Elements/Direct’s surfacing 
tools under the same umbrella. Those surfacing tools, however, 
have already been captured under a different group — some twice. 
What we’re left with is Loft, Sweep, and Helix in the Ribbon 
Modeling Model ...More overflow menu. 
Loft. The Loft tool can be very elaborate. At it’s heart, Loft will 
create a freeform model by forming a smooth transition between 
at least two profiles. 
 The Loft tool is drawing lines between the profiles from ver-
tex to matching vertex, so the number of vertices need to match-
up. You also provide a Match Line (Create ML) for that purpose. 
This ML represents the first match-up between vertices. The tool 
assumes the rest. Not only do you need to provide these things, 
they need to be wrapped-up in a nice package called a Workplane 
Set before you can begin your loft. Ribbon Structure 
Workplane ...More Workplane Set. Once you have 
everything together, execute your Loft Add and most of the 
options are defaulted for you. 
 Use Add Tan to add tangency controls to the vertices 
before lofting. The dialogue allows you to adjust the refer-
ences and weighting of the tangency as well. All this ad-
justs how the lines connecting your profiles are drawn. Do 
they shoot directly from one vertex to another, or do they bow 
and curve to achieve tangency or curvature continuity with 
existing parts or faces? Try adding multiple workplanes to your 
set and rotating them in different directions. 
Sweep. Only one workplane and one spline 
curve to worry about in a Sweep. The profile(s) from 
the workplane is swept along the spline curve (the 
Spine) to create a freeform part. 
Helix. The Helix operation sweeps one 
profile about an axis (see Right-Hand Rule) 
in order to create a helical part. Adjust the 
pitch and number of turns in the dialogue 
and click the Preview until your helix is per-
fect before completing the operation. 
2D SKETCHING WITH SPLINES 
2D Splines come in two flavors; Interpo-
lation and Control. In an interpolation 
spline, you define a series of points through 
which the curve passes exactly through. 
With control splines, the shape of the spline 
is influenced by a dynamically created con-
trol polygon formed by control points against 
the spline curvature. 
3D CURVES AND POINTS 
Sketching in 3D space can be an unset-
tling proposition. When it comes down to it, 
what you’re doing is defining points in 3 
axes. See your tools. They can be found 
under the 3D Geometry tab in your ribbon. 
 The different commands like line, cir-
cle, spline, or arc are all just doing different 
things with the points you define. Sohow do 
you define points in 3D space? 
 The trick is really the first 
vertex. From then on, each sub-
sequent point can reference the 
previously created one. Rather 
than simply clicking on the 
screen, try defining coordinates with the 
user input line or capitalizing on the Catch 
tool to grab an existing 3D reference for 
your first point. Each tool will have its own 
snap helpers too. Face, edge, and axis, for 
example. If you have nothing to snap to, you 
can use the 3D CoPilot helper for your first 
point. 
It may take a little getting 
use to, but this u, v, and w axis 
widget represents the local 
coordinates of each point. Click on its axes 
or planes to restrict movement and select 
your target location. This same widget is 
then used for each subsequent point. From 
then on it’s much like sketching in 2D. 
ALERT: If you create prismatic geometry with 
splines like straight lines or circles, your part my 
later appear corrupt. Use the right tool for the 
job to avoid more work down the road. 
ALERT: There must always be a gap, even a mi-
cro-inch, between each turn of your helix. If the 
turns touch, the intersection will cause an error. 
BEST PRACTICE: Use Containers to group all of your workplanes, 
workplane set, and match line together for future reference. 
Note: Cursor icon may change to have 3 dots 
under it during these commands to indi-
cate a command specific right-click menu. 
QUICK REFERENCE GUIDE 
 17 
 MODELING: ADVANCED MODELING 
Modeling 
CREATING 2D PROFILES FROM 2D AND 3D GEOMETRY 
There are a series of projection tools available for the purpose 
of speeding your 2D profile creation. With the typical tool set, 
you’d need to grab references to 2D or 3D geometry and draw over 
them, much in the same way that you might create construction 
geometry and use the Overdraw command to trace what you want 
to keep. Creo Elements/Direct has done away with the absolute 
need for Overdraw and likewise done away with the need to trace 
already existing 2D and 3D geometry into new profiles. These 
commands can be found in the Project drop-down in the Draw 
command group of the Modeling tab. Ribbon Modeling 
Project. 
The distinction between Construction and Geometry com-
mands defines how the resulting projection will appear in your 
workplane; as construction lines or 2D geometry. The Face and Edge commands don’t have 
command details, so you wouldn’t be able to toggle between the two as if they were part of 
the same command. 
Project Face, 2D Edge, and 3D Edge do as their namesakes suggest. They project the 
geometry of a face, 2D edge, or 3D edge respectively onto the target workplane. The Gen-
eral command does have a command dialogue and allows for a bit more control over your 
projection options. Cross Section projects a cross section onto a target workplane(s) wher-
ever it intersect a part(s), while Outline will project only the outline of a part or face(s) onto 
the intersecting workplane. 
Along the same line, there are two combo commands that will 
create a workplane and create 2D profiles for you at the same time. 
The projected profile works more like a cross section than an out-
line. Internal features that intersect the workplane are projected as 
well. New WP on Face and Project Real and New WP on Face and 
Project Constr don’t have command details either. Just activate the 
command and select a face. You can find these commands on the 
Workplane dropdown in your Ribbon Modeling Workplane. 
 
BEST PRACTICE: Commands can be separated like this to make it easier to access the 
exact function you want on a keyboard shortcut or abbreviation. If the commands were 
consolidated, your shortcut would only get you to a details dialogue that you’d then need 
to manually, or through a mini toolbar, adjust for your needs. Try assigning common 
commands in File Customize to speed your work. 
The 3D Surface Tools group is located 
under the 3D Geometry tab along with 3D 
Curve and 3D Point command groups. 
These tools have more of a repair and recov-
er feel to them. Granted, you can get ex-
tremely advanced surfaces by using 3D 
Curves and Insert Face, but mostly the tool-
set is basic in its face operations; Can be 
much less organic and much more rigid in 
execution than what you would see in the 
Advanced Surfacing Module. 
 Face Parts are made-up of individual 
faces that do not form a solid body. This 
allows you to design complex models by 
adding individual surfaces to existing de-
signs or starting new ones from scratch. 
Once the faces converge into a closed shell, 
Creo Elements/Direct will automatically 
convert the face part into a solid part. 
 Insert Face is arguably the most ad-
vanced tool in the group. Insert Face cre-
ates faces by interpolating from a set of 
boundary curves or edges. If you’re using 
3D elements (Collectively occupying more 
than one plane in 3D space), there’s a limit 
of six edges. On a 2D plane, there’s no 
limit. Many of the subsequent tool func-
tions can be achieved with an Insert Face. 
 
 Grow Surface will grow a face(s) in the 
direction of the edge(s) you choose. This 
growth will happen infinitely, so you must 
define boundaries in the way of parts, faces, 
planes, or surfaces to limit your growth. 
Otherwise the command will likely fail. 
 Reintersect Faces will grow several 
faces or edges at once using their own inter-
section as your boundary definition. Best 
used to close gaps between neighboring 
faces. 
 Untrim is, in essence, a reverse engi-
neering aid. It creates a new face part rep-
resenting the geometry that was used to 
trim away at your selected geometry. 
 Thicken creates a solid part from a 
face part by creating an offset copy of the 
face(s) and growing side-surfaces between 
the original and the copy. 
 Show Gaps highlights unbound edges 
in a face part. These edges mean the differ-
ences between a face part and a solid part. 
 Gather Faces allows you to select 
faces from a solid part and copy them to a 
new face part. Very similar to the Copy com-
mand, but without the position option. 
 Delete Face will poke holes in your 
solid part turning it in to a face part or allow 
you to take your face part to pieces one face 
at a time. 
 Flip Faces will flip the direction of the 
normal on a given face or set of faces. 
 Trim will use one face as a boundary 
(Tool Face)to cut another (Blank Face(s)). 
QUICK REFERENCE GUIDE 
 18 
 MODELING: ADVANCED MODELING 
Modeling 
PATTERNS 
Patterns can be accessed from the 
Feature tab as well. 
You’re able to pattern 
Machining features, 
Mold Design features, or 
Face Set features. You 
can also create patterns 
of parts within the same 
assembly. 
Modify the pattern 
at any time by excluding 
elements or include ele-
ments that were previ-
ously excluded. It can’t be deleted with the 
delete key or a right-click option. Use the 
delete command from the Pattern group. 
Geometry in a pattern is shared out 
from the initial feature. If you make chang-
es to any of the features in the pattern, all of 
the other features in the pattern have the 
potential to change to match. You can use 
Modify to restore the altered pattern mem-
ber to its original, or use the OwnPat check-
box to propagate the changes to the pattern. 
Defining a pattern can depend on the 
type of pattern, but generally the definition 
shares some common characteristics. 
Linear Direction. You need 1 for a Line-
ar pattern and Radial Grid, and 2 for a 
Linear Grid. This uses the 3D CoPIlot 
widget to define which way these pat-
terns point. 
The Number of pattern members is tied 
to the direction. In a grid, if you define 4 
in one direction and 4 in another, you’ll 
have 16 total pattern members. In non-
grid patterns, the number is exactly how 
many total patternmembers you’ll end 
up with. A Free pattern’s members are add-
ed one at a time. 
The Start Position defines where the 
pattern should begin. Normally, the start 
position is the origin of the originating fea-
ture, but this can be offset according to your 
needs. 
Your Distance can be defined as the 
distance between each pattern member in a 
given direction, or as the Total Distance in a 
given direction. In either case, the members 
are evenly distributed. 
In Radial patterns, you must define an 
Axis. Normally this is the center of your 
source feature, but can be changed. The 
Radius determines how far out from your 
start position the pattern members will start 
to occur in a circular pattern. The Angle 
determines how much space is between 
each pattern member. Similarly to the line-
ar distance, you can define this as a gap or 
as the Total Angle to be covered by the pat-
tern. 
FEATURES 
A Feature is a set of faces grouped 
together and saved in a named container in 
the structure browser under the given part. 
They can be used as a method for selec-
tion, can contain information for down-
stream processes, and are also used to 
create patterns. 
There are two variations on the Fea-
ture functionality. You can create a Face 
Set Feature of four specific geometry types 
or a User Defined Feature for 
everything else. The difference 
is that a Face Set Feature can 
be patterned while a User De-
fined Feature can not. 
A feature can consist of any number of 
3D elements but they must all belong to the 
same part. 3D elements are recognized as 
edges, vertices, or faces. You can access 
these feature commands and a few more 
on the Feature tab of your ribbon. 
Your geometry does 
not need to match the 
icon exactly. The icon for 
each of the four Face Set 
Features is strictly convey-
ing a simple set of re-
quirements for each. 
If your feature needs to change, you 
can alter the type of Face Set Feature you’ve 
selected. Use the Ex-
change command in 
the More drop-down to 
select a new type. 
When defining a 
Face Set Feature, you’ll have 3 attributes 
automatically defined for you. The local 
coordinates for the feature, the main direc-
tion used for a manufacturing process, and 
the secondary direction. 
 
 
 
Ref. Pos. This local coordinate system 
can have a big impact on future patterns. 
Consider a boss whose diameter changes 
down the road. If the local coordinate sys-
tem had not been centered, the resulting 
pattern would be affected by a diameter 
change. 
MainDir. A manufacturing process 
would be a drill, mill, punch, etc. This can 
help define which side of the part should be 
worked during manufacturing. 
StartDir. Should not be parallel to 
MainDir. Helps define where a machining 
process should begin. 
TIP: A User Defined Feature can still be patterned 
using Copy Face and Paste Face commands. You 
just don’t have the creation and redefinition op-
tions available for pattern features. 
TIP: When making changes to features, be sure to 
use the correct Modify command. There are 3 on 
the Feature tab and they’re not interchangeable. 
 
TIP: Use the TAB key to flip a direction widget 
from the 3D CoPilot. 
QUICK REFERENCE GUIDE 
 19 
 MODULES: MACHINING 
Modules 
Creo Elements/Direct Machining is an 
advisor module. It assists during the de-
sign phase by allowing easy specification of 
common machining features, providing 
easy modification of those features, and by 
providing advice about machining opera-
tions. Machining assists further when cre-
ating documentation by providing methods 
to transfer dimensional tolerances into the 
annotation module in a streamlined pro-
cess. You can even transfer technical infor-
mation into select CAM systems. 
Creating Holes. Click on the hole of the 
desired type (Through, Tapped, or Blind) for 
the placement dialogue. Fill the yellow dia-
logue boxes and complete your new feature. 
Notice that the hole is created as a feature 
in the structure browser and matching anno-
tation was generated. 
During the feature dia-
logue step, you can click 
Show Image for a detailed 
image explaining your hole 
options. 
 Also during feature specification, the 
advisor component kicks in. These checks 
are based on general rules and can be 
changed using the CED Integration Kit. 
Modifying Holes. Simply right-click on 
the hole feature in the browser and select 
modify to go right back into the hole dia-
logue. 
Hole Patterns. Create a New Pattern 
from the Feature tab and choose the hole 
feature from the 3D viewport as the source. 
You can create linear, linear grid, radial, 
radial grid, or free patterns in this manner. 
The pattern feature is fully parameterized 
and can be modified just as easily as the 
hole feature itself. 
 
Adding Threads to Cylinders. The ma-
chining module can also 
add thread features to ex-
isting cylinders for the crea-
tion of bolt or screw mod-
els. Choose one of the 
outer threads from the machining options 
and select your bolt or screw’s cylinder as 
the target face. 
Specifying Tolerances. You can add 
tolerances to hole features. By default, 
they’re appended to the dimension label, 
not the note hole 
note text. You 
can add Upper/
Lower, Plus/
Minus, Limits, or 
ISO. Inside the 
hole dialogue, 
click on the Show 
T&Q button for the extended tolerance op-
tions to appear under Diameter Tol. 
 
Specifying Quality. Surface quality can 
be assigned to all machining features. 
These are best used in the 2D drawing from 
the information stored in the 3D note or 
further downstream in manufacturing 
through the machining output reports. Also 
under the Show 
T&Q options, 
click on the Side 
Quality button for 
your options. 
 Machining Settings. Under File 
Settings Machining, you can make quick 
adjustments to common controls for ma-
chining features. 
Data Table Customization. A more 
permanent form of adjustment is achieved 
with data table customization. This method 
allows you to customize the machining envi-
ronment to suit your design needs exactly. 
You can create custom holes, defaults, 
change advisor validations, and more. This 
is typically done by your CAD administrator 
through the use of the CED Integration Kit. 
CED Integration Kit. The kit itself is a 
collection of tools typically used to program 
add-on applications for CED. Making chang-
es with the Integration Kit requires a thor-
ough understanding of CED, some basic 
programming skills, and a basic knowledge 
of the Common Lisp Programming Lan-
guage. 
 
Activate Machining FileModulesMachining Access Machining RibbonFeatureMachining 
NOTE: Settings changed in this way work for 
your current session only unless you save the 
settings to an environment file. 
ALERT: Changes made through the Integra-
tion Kit are not guaranteed to work with fu-
ture releases of Creo Elements/Direct. 
BEST PRACTICE: Adding threads as a feature 
is usually preferable over an actual helix. 
Conserve your graphics capability for your 
design imperatives. 
QUICK REFERENCE GUIDE 
 20 
 MODULES: SURFACING 
Modules 
The Surfacing Module is a much more 
organic set of surfacing tools than are 
available out-of-the-box. Each command 
takes much more time and dedication to 
master, but the resulting capability and 
possibilities are well worth it. 
 
 Skin is like Insert Face times ten. 
You’re inserting a face via 2D or 3D curves 
or edges like Insert Face, but here you can 
use curves inside a mesh as guides in addi-
tion to the boundary curves. This apparent-
ly simple change opens the door to a wide 
range of capability, command options, opti-
mization, and built-in surface analysis 
tools. Many of the subsequent tool func-
tions can be achieved with a Skin.Advanced Sweep adds three new 
additions over normal 
Sweep; The option to 
create face parts, the 
use of any collection 
of edges as the sweep 
profile, and the use of 
a second guiding 
curve for the sweep. 
 
 Guided Loft is a marriage of the 
Sweep and Loft tools. A Sweep allows you 
to take a single profile and sweep it along a 
single guiding line or spline. Loft will take a 
series of profiles and draw lines between 
them to create a solid body. Guided Loft 
combines them by removing the need for 
multiple profiles, adding a line or spline as 
a guide for your loft, and automatically add-
ing helper profiles along the path. 
 
 Cap creates a 
freeform cap on a part 
using a Cap Point and 
looped edges. 
 
 Face Round. Like a 3D fillet between 
faces, Face Round creates a chain of 
rounded faces to connect two face part 
sets tangentially or curvature continuously. 
 
 Bridge. A quick way 
to fill the gap between two 
faces. Does not need to 
be fully bounded. Just se-
lect two edges or sets of 
edges you want to bridge. 
The connection can be 
made tangential and the 
curvature weighted. 
 
 Extrude Edges. Similar to Grow Sur-
face, but here you’re creating a new face 
part and can change the direction and 
length of growth with the 3D CoPilot. 
 
 Extrude Face Part. Similar to Thick-
en, but you’re not creating a uniform thick-
ness offset. You’re extruding directly from 
the original face part to create a solid part. 
 
 Surface Editor. An extremely power-
ful surface tool used to control surface 
contours with a wire model and parametric-
like constraints. 
 Smooth Surface. 
Easily analyze and 
smooth surface transi-
tions with color coded 
feedback and real time 
surface analysis. 
 
 Modify Surface. Quickly and easily 
manipulate custom surface meshes to cre-
ate complex surfaces. A favorite tool for 
making bold surface changes. You build 
your custom mesh by click points on the 
surface. The 
tool creates 
intersection 
lines that you 
can grab and 
manipulate. 
 Offset Face Part. Similar to Offset, 
this tool will offset a face part normal to the 
original faces while making adjustments to 
the face geometry based on the offset dis-
tance (similar to the adjustments a Thicken 
might make). 
 
 Adjust Faces is used to work the tran-
sition between faces. Typically, it’s a good 
idea to create good face transitions during 
design, but Adjust Faces can be used to 
repair poor connections. 
Analysis. Skin, Guided Loft, Cap, 
Bridge, Smooth Surface, Modify Surface, 
and Adjust Faces have built-in real-time 
surface analysis capability. Once Surfacing 
is activated, you can also access these 
tools under the Analysis tab. 
The Surface Analysis tool 
will analyze the quality and 
curvature of a surface or sur-
face transitions. You can also 
check min-max radius values. 
Types are Gaussian curvature, Mean curva-
ture, and Zebra stripes. 
Angle Analysis will deter-
mine the maximum angle 
along an edge between two 
faces along the intersection. 
Activate Surfacing Module FileModulesSurfacing Access Surfacing Module RibbonSurfacing 
ALERT: Surface Editor requires the Parametrics 
module as well as the Surfacing module. 
QUICK REFERENCE GUIDE 
 21 
 MODULES: BASIC SHEETS 
Modules 
Basic Sheets is a free module with a 
small, but surprisingly effective set of sheet 
metal creation and modification tools. You 
can start using sheets by either creating a 
new piece of sheet metal from scratch (New 
By Outline) or by using these sheet metal 
operations on any model that would meet 
the physical requirements to be manufac-
tured as sheet metal. Keep in mind that 
using this module does not preclude you 
from using standard modeling commands. 
By combining the techniques, though, you 
run the risk of creating a part that can no 
longer be modified by the Basic Sheet com-
mands. For example, a non-uniform thick-
ness part will eliminate or hamper most of 
your options. 
New By Outline. Create a brand new 
sheet metal part from an active workplane 
and a sketched closed region. The dialogue 
box will allow you to choose a material which 
will derive your sheet thickness for you. 
Material. The Attach Material com-
mand can initiate or modify the material 
definition of your sheet metal part. It brings 
up a list of thicknesses from the Basic Shop. 
Careful when deleting these thicknesses. 
Adding them back is not as easy. 
 
Unfold and Refold. Simple, but essen-
tial in sheet metal design. These com-
mands will do just as their namesake sug-
gests. They’ll unfold or refold your entire 
sheet metal part. Simply select the com-
mand and choose the face(s) that are to 
remain stationary during the process. 
Fold/Unfold. This single command will 
recognize and toggle the bend status of any 
given bend. It doesn’t matter if the bend 
was created with Basic Sheets or some oth-
er process. 
Create Bends and Modify Bends. You 
could create the entire sheet metal part in 
the flat, then use bends to fold it up. To 
create a bend, you’ll need an active work-
plane with a sketched line on it. Your line 
is extrapolated infinitely and intersected 
with your sheet metal part for bending. 
Breaks in the sheet metal are recognized 
so if you want multiple flanges to bend, 
make sure your sketched line crosses into 
each if they’re on the same plane. 
Bend Animation. Visually simulate the 
folding and unfolding of a bend. You can 
change angle between each step in the 
animation. Step in and out of the anima-
tion one frame at a time. Finally export 
your animation as an AVI. 
Add Lip. Once you have a 
sheet metal part, you’ll need to 
start designing with it. Lip is a de-
ceptively simple command with a 
significant amount of complexity 
tied into it. On the simple side, just 
grab an edge, type in a length, and 
Lip it. Done. On the complex side, 
there’s a myriad of options availa-
ble for the Lip command. 
L/R AutoMiter. Turn this on to 
detect a miter situation. If detect-
ed, the system retrieves as many 
parameters as possible. 
Left/Right Lip. Select corner 
options. The green area is the new 
lip to be added. 
Left/Right Angle/Dist. Angle 
in/out from and Distance from 
each end reference. 
Connection. Options to pre-
vent material deformation where 
the lip connects to the original 
sheet. Defaults to automatic for 
each end. 
Activate Basic Sheets Module FileModulesBasic Sheets Access Basic Sheets Module RibbonSheets 
 
 
 
 
 
 
 
 
Add Lip 
ALERT: Once a lip is created, it’s 
treated like any other bend. You 
won’t get back the same dialogue 
when making changes. 
 
 
 
Angle 
Distance 
QUICK REFERENCE GUIDE 
 22 
 ASSEMBLIES: BUILDING ASSEMBLY STRUCTURES 
Assemblies 
ASSEMBLY STRUCTURES 
Assembly structure refers to a logical collection of parts and assemblies in a hierar-
chical structure. In Creo Elements/Direct, the assembly structure is visually represented in 
the Structure Browser. Each individual assembly in CED is a simple Bill of Material (BoM) 
that acts as a container for parts and sub-assemblies. You can manage assembly member-
ship in the structure browser through a drag-and-drop interface. Assembly tools can be 
found in the Structure tab. 
GLOBAL AND LOCAL COORDINATES 
Creo Elements/Direct uses two 3D coordinate systems; global (X, Y, Z) and local (U, V, 
W). While there is only one global, all children of the world of CED have their own local coor-
dinate systems. It follows that an assembly container has its own local 3D coordinate sys-
tem. Further, each part and assembly within can be considered to have a relative position 
to the parent coordinates. Likewise, each element in the hierarchy of the Structure Browsercan be considered to have a relative position to its parent up to the root of the hierarchy 
where the global coordinate system is the parent. 
 
STRUCTURE BROWSER 
The Structure Browser lists all 3D ob-
jects and elements in a hierarchical struc-
ture which illustrates their relationships to 
each other. Check and uncheck individual 
items to show or hide them in the viewport. 
Use Ctrl+click or Shift+click to select multi-
ple items. You can also right-click for a 
menu of actions to execute against the se-
lected item(s). Click the plus or minus signs 
to show or hide the children of a container 
in the hierarchy display of the browser. 
NEW ASSEMBLIES 
Using New Assembly will cre-
ate the container in the structure 
browser. The dialogue box asks 
for the name of the new assem-
bly, the model name, and the 
owner. Adding an owner allows 
you to avoid the drag-and-drop by starting 
the assembly under another container. The 
model name is optional. It refers to the 
name of the Contents Data container. 
 
Global Container (X,Y,Z) 
/a1 Container. Local U,V,W relative to Global XYZ 
Local U,V,W Relative to /a1 
/a2 Container. Local U,V,W relative to /a1 
Local U,V,W Relative to Global X,Y,Z 
Local U,V,W Relative to /a2 
POSITIONING PARTS 
You can position a part by using the Position command from the ribbon UI, by double 
left-clicking the part in your structure browser and clicking the Position command from the 
mini toolbar, or by the right-click context menu in 
the 3D viewport. Dynamic and Mate Align are only 
two of the fifteen methods available for positioning. 
Dynamic position is the default, and allows you to use the 3D 
CoPilot widget to position your part. 
The Mate Align option opens another set of options with which 
you can position a part by face relationships. 
Align Axis is another very important placement option under Ma-
te Align. Especially useful when employing Coordinate System fea-
tures to position complex parts. (By Ref CS works well there too.) 
 
 
TIP: You can also initiate the Position com-
mand by left-clicking on any vertex in a part. 
BEST PRACTICE: Containers can help organize workplanes or other useful objects in the Structure 
Browser. Structure Parts & Assemblies More Tools New Container 
ALERT: Positioning a part does not constrain the part permanently. Any 
implied constraints are only used to aid in placement and are temporary. 
The part is free to be moved in any direction after positioning. 
Aligned Mated 
Parallel Parallel 
QUICK REFERENCE GUIDE 
 23 
 ASSEMBLIES: CONTAINERS, COPY, SHARE, AND INSTANCING 
Assemblies 
COPY VS. SHARE 
It’s best to use Share for any part or assembly that you’re using more than once rather 
than making a copy. Making a copy will duplicate the part or assembly entirely. Sharing 
does not create a copy, but an instance of the original. This will ensure that any modifica-
tions you make to the part or assembly Contents Data are automatically reflected in all oth-
er shared instances (Instance Data). This applies to geometry as well as changes in the 
base settings and other shareable attributes. Any previously shared part or assembly can 
be unshared. This will, in effect, create copies where once were only instances. 
SELECTIVE INSTANCING 
Sharing is a huge time saver and it’s also just good practice to have 
one master part that’s shared when possible. Still, there are some situ-
ations where the inherent association between shared parts and assem-
blies can become a problem. For example, if you wanted to move a bolt 
in a set of shared assemblies independently from the others without 
affecting the BoM. You might selectively unshared the instance and 
make your changes. 
Unshare and select the bolt in question. Chose a new name if you 
have one and the new context. Notice in the images below that the Sel 
Inst Context is set to the container above the shared parts. The default 
is one container upwards in the hierarchy where the selected instance has an impact, but 
you can change this manually in the Unshare command dialogue box. 
Use Reshare when you’ve changed your mind or circumstances require the reversal of 
your previous Unshare. The part or subassembly will revert back to its original state. 
The Cleanup command is used when a selective instance exists, but all the other 
shares have been deleted or unshared. There would be nothing to revert back to if Reshare 
was used. The Cleanup command effectively removes any sharing baggage and makes the 
selective instance independent. This command will not work if there are still shares that 
would be affected by the removal of the share data. 
Master. Selective instancing can cause issues with assembly instances that are shown 
in the documentation. Master allows you to specify which assembly share is to be used 
when computing view geometry. 
 
 
Content 
Data 
Instance 
Data 
Content 
Data 
Instance 
Data 
Content 
Data 
Instance 
Data 
Content 
Data 
Instance 
Data 
Instance 
Data 
When you create a share, the system automatically creates a folder to contain share 
data and places your newly shared items underneath. Creo Elements/Direct has no dis-
tinction between the original part and the shared instances. If you change one, it changes 
them all. However, each instance can have its own part 
and instance data while remaining an instance. 
For example, you can change the position, name, 
and part colors of instances. To change part instance 
colors, examine the properties of any of the shared 
parts. The dialogue box shows appearance properties 
for Instances separately from Base properties. A
ss
y_
In
sta
nc
e1
 
As
sy
_In
sta
nc
e2
 
View Details 
CONTAINERS 
You can find the New Container command under the Structure tab in the 
Part & Assembly group’s More overflow menu. A container is a structural or-
ganization tool. They can be used to hold models, assemblies, and work-
planes. They are particularly useful for organizing complex geometry modification elements. 
None of this reference data or geometry will be transferred to Annotation so these building 
blocks will not appear in the drawing. Without a container, you’d likely need to manually 
remove these references from each drawing view. 
QUICK REFERENCE GUIDE 
 24 
 
ADVANCED ASSEMBLIES: CLIPPING PLANES, STOCK/FINISH, 
 AND COORDINATE SYSTEMS 
Assemblies 
CLIPPING PLANES 
A clipping plane allows you to look through a part or assembly 
as if you’d cut away from them along a plane to reveal the fea-
tures, parts, or assemblies behind. A familiarity with clipping 
planes will allow you to navigate and inspect your designs much 
more effectively. You can find the clipping plane commands on 
the View tab in the Clipping group. 
Once defined, a clipping plane remains in your 
design as a clipping plane feature that can then be 
activated or deactivated as needed. You can view 
particularly troublesome areas and access their 
clipping planes whenever needed. 
A single clipping plane feature can contain many clipping 
planes. In fact, you can not have multiple clipping plane features 
active at once. Only one per viewport active. So, if you want to 
clip from multiple directions, you’ll need to define each plane in a 
single feature’s dialogue box. Up to six total clipping planes can 
interact with each other in a single feature. 
To change which parts will be clipped and which will not, use the Targets command. 
Your selection will define the targets for all clipping features in your model. To change how 
your clipping planes are viewed in the viewport, change the viewport show properties via a 
right-click Show Properties, or change the clipping plane settings. Use the settings button 
on the Clipping group in the ribbon UI. 
 
STOCK/FINISH 
A stock finish relationship does not propagatechanges from one member to another like 
a share relationship. The idea is that you may have a situation where you have a stock part 
that is somehow altered in its finished form. Color, extra holes, draft, etc. Maybe you actually 
have a literal stock/finish relationship where you buy copper bar stock and cut your own fin-
ished lengths. The Stock/Finish operation will create a relationship between the two parts to 
aid the process of managing different related product states. 
 A stock part can have many finished parts, but a finished part can only come from one 
stock piece. However, you can also chain the effect. So the finished product from one opera-
tion can be come the stock for another finished piece. 
TIP: You can also activate/deactivate 
clipping planes by double-clicking 
them in the Structure Browser. 
Finish_Cut2 
Bar_Stock Finish_Hole 
Finish_Cut1 
COORDINATE SYSTEMS 
When dealing with advanced assemblies, it can sometimes become 
difficult to find handles or attachment points between geometry. One way 
to alleviate this issue is to add custom coordinate systems to your parts or 
assemblies. You can line them up to your part or assembly in whatever 
direction suits your needs and reference them for movement or assembly placement. These 
coordinate systems will attach themselves to their owner and can therefore be shown or hid-
den like any other object in the Structure Browser. 
Create a new Coordinate System from the command group of the 
same name in the Structure tab. You’ll need an 
owner, name, and position. They can always be 
renamed and repositioned as well. For your visu-
alization needs, the Coordinate Systems can be 
resized and recolored. 
TIP: You can always snap to the center of a 2D circular feature or 3D spherical one by holding down 
Shift+Ctrl. You’ll need to press Shift+Ctrl regardless of your 2D or 3D CoPilot snap key settings. 
TIP: Coordinate Systems can be extremely helpful for advanced 
positioning. Try adding them to complex objects. 
TIP: You can manipulate geometry while clipping 
planes are active. Try modeling with clipping on. 
TIP: You can now create new workplanes off of existing clipping planes. This is a com-
mand option in the dialogue box for a new workplane and can also be accessed via the 
context menu (right-click in viewport). 
QUICK REFERENCE GUIDE 
 25 
 ADVANCED ASSEMBLIES: CONFIGURATIONS AND EXPLISIONS 
Assemblies 
CONFIGURATIONS 
A configurations is used to store the positions of parts, what’s hidden or shown in the 
viewport, and different camera direction through various stages of an assembly. To create 
a configuration you must have an assembly, but the configuration itself can be owned by an 
assembly that’s further up the hierarchy if needed. The 
owner of the configuration can not be the root of the 
structure browser. Configuration operations can be 
found in the Structure tab in the Configurations group. 
Once you’ve created your configuration, making 
changes relies upon your activation or deactivation of 
the configuration. Use the Act/Deact commands or 
simply double click your configuration in the Structure 
Browser. Once it’s active, any changes that you make 
to the assembly or any subassemblies underneath the 
configuration’s owner are recorded by the configuration. Toggle Act/Deact to see your parts 
smoothly float in and out of the various positions set by each of your custom configurations. 
If you do not move a part while your configuration is active, then no positional infor-
mation is stored for that part. If you want to make sure positional informational is stored, 
click the Hold command. This can be important especially when considering how subas-
sembly components may get moved around in your design. 
When creating an assembly process, it can be convenient to Copy the previous configu-
ration as a starting point. To capture camera position or draw list, use the right-click menu 
on your configuration. This information is not automatically stored like part position. You 
can even make changes to this information without the configuration being active. Use 
Highlight to see which parts are being controlled by the current configuration. 
If you make a mistake or want to remove some of the data you’ve captured, use Re-
move Data. The dialogue box will ask if you want to move positioning, camera, or drawlist 
information. Of course, you can do away with a configuration entirely with the Delete com-
mand or by right-click delete. To show multiple configurations at the same time, use the 
Multiple Positions command. 
EXPLOSIONS 
An Explosion is the most common kind of Configuration. You can build from scratch or 
change an existing configuration into an explosion. This is also the same method used to 
modify existing explosions since an explosion is considered just another configuration when 
you’re done creating it. The command will take your assembly and blow it apart. You de-
cide how it explodes and how far. Sounds fun, doesn’t it? 
To create an explosion, select Explode from the Configurations command group in the 
Structure tab. Choose your configuration or create a new one. The One Level check box 
indicates if you want the subassemblies to behave as single parts of if you want the individ-
ual parts to move as well. The Scale determines how far the parts will be moved from the 
explosion center. In the case of a Cylindrical explosion, you’ll have an Axial and Radial 
Scale. The Show Move Feedback checkbox determines if you’ll have a visual representation 
of the movement or not. This is shown as green lines extending from original positions to 
ending positions. The movement references are temporary and will disappear as soon as 
you’re done configuring the explosion. 
Align Axes. This mode constrains objects with coincident axial 
faces to explode along their common axes. Objects without are ex-
ploded spherically. 
Spherical. A spherical explosion will move all objects in all direc-
tions away from the explosion center. 
Cylindrical. Move objects away from an axis radially and axially. 
You can set the axial and radial scales of movement separately in a 
cylindrical explosion. 
By Direction. You’re shaping the direction of the explosion. An 
explosion is typically spherical; where everything radiates 
away from the explosion center. This will move objects 
away from the explosion center as well, but only in the di-
rection you specify only. 
Pos Dynamic. If none of the default explosion types are working for you, you can al-
ways manually position the parts. 
 
 
ALERT: You should not use the Formations goodie. The Configurations feature replaces its function-
ality. Use the Convert command to upgrade any Formations you may have in existing assemblies. 
NOTE: Please note that each Explosion feature can have a series of 
explosions inside. The explode and back buttons inside the dialogue box 
allow you to work through each explosion individually. 
ALERT: Configurations do NOT change the original position of your assembly. Activate and Deacti-
vate configurations to see your assembly in different positions/configurations. The original remains 
the same throughout. 
QUICK REFERENCE GUIDE 
 26 
 ADVANCED ASSEMBLIES: CLASH ANALYSIS 
Assemblies 
CREATE CLASH ANALYSIS 
 The Create Analysis command will cre-
ate a Clash Analysis object in your structure 
browser. This object will contain the 
parameters for your analy-
sis and any results you may 
have calculated. If the icon 
is green it means 
you’re analysis is out of 
date. 
Once it’s been created, 
you can always modify, 
rename, delete, calculate, 
clear issues, and bring up 
the Clash Issue Browser 
from right-click commands 
on the object in your Struc-
ture Browser or from com-
mands in the ribbon UI. 
When you execute the Cal-
culate option, itwill run 
through your assembly to discover if there are interferences 
based on the parameters you set in the definition of the 
clash analysis. Once you’ve selected what will be analyzed 
and where the analysis will reside, you can change options 
like ignoring press fit parts, ignore parts from the 3D library, 
ignore threaded parts and holes, specify specific clearance, 
and exclude parts from the analysis. 
A Clash Analysis must be owned by an assembly and 
not by the root “/” or a selective instance of the assembly. 
If the selective instance is created after the analysis, your 
icon in the Structure Browser will turn red. This indi-
cates an invalid analysis. To repair the situation, attach the 
Clash Analysis to a valid owner and recalculate. When the 
icon is yellow it means that the assembly is only par-
tially loaded, might contain lightweight parts, or the state of 
the analysis is undefined. 
 
CLASH ANALYSIS ISSUE BROWSER 
 Once you run the analysis, the Clash Analysis Issue 
Browser will show up. If you close it, you can always re-
summon it with the right-click command in the Structure 
Browser. This is where you view your clash results. The 
issues are listed numerically in the browser and can be 
searched, filtered, and sorted for your easy perusal. 
 Just like the Structure Browser, you can define very 
complex searches through the binoculars icon. It will allow 
you to define a list of custom criteria and store those 
searches for later use. Filtering is much the same. 
Once you have the list narrowed, you can right-click on 
individual issues for a list of commands. Draw Only will 
remove everything from your viewport but the parts brought 
into question by the issue. Draw Only in new VP will do the 
same as Draw Only, but create a new viewport to view the 
parts in. Recalculate Issue will bring up a command dia-
logue for a single clash and an auxiliary viewport with your 
issue specific parts in it. Search Clash Analysis in Structure 
will find the clash analysis in the Structure Browser (in case 
you’ve lost it). Search Parts in Structure will find your issue 
specific parts in the Structure Browser. The Properties of 
the Issue are also available and provide a detailed status 
and resolution pop-up. 
 
RESOLVING CLASH RESULTS 
There are only three ways to 
resolve a clash. The most obvi-
ous being fix the problem. The 
Clash Analysis tools provide a 
number of methods for finding 
and refining your models by giv-
ing you easy access and detailed 
information about each issue. In particular, Recalculate 
Issue will give you the Draw Only in New VP, but with a trans-
lucent model that highlights the volume of intersection in 
red. The clash dialogue box that pops-up from the Recalcu-
late Issue will give you quick access to methods for redefin-
ing the analysis for that specific issue. Change the status to 
“Modified” in the properties pop-up when your changes are 
complete. 
The second way is to accept and ignore the problem. 
You will definitely run into situations where a clash is inten-
tional. Press fits, interference fits, etc. Add a note to the 
issue’s properties and select “Accepted” in the status 
dropdown. 
The third and final way to resolve a clash result is to 
ignore it. Yes, you can mark the issue as “Conditional Open” 
or “Conditional Accepted” and write a note for posterity de-
scribing why this issue was unavoidable or when it will be 
revisited. 
QUICK REFERENCE GUIDE 
 27 
 ANNOTATIONS: ANNOTATION APPLICATION 
Annotations 
APPLICATION: ANNOTATION 
The Annotation application in Creo Elements/Direct is the 2D tool used for creating 
drawings from 3D designs. To use Annotation, you can select File Modules and find the 
Applications submenu. Put a check in the Annotation check box. Once you’ve done that, 
you can switch between Modeling and Annotation by going to the Applications tab of your 
ribbon UI. Toggle between the applications as needed. Annotation runs in parallel with 
Modeling. 
 
 
Look and Feel. The Annotations application has the same look and feel of Creo Ele-
ments/Direct Modeling. It has the same menu and dialogue functions — Even the same 
interface layout and navigation as the Modeling application. When toggling between the 
two, it’s seamless enough to be considered the same application. 
Associativity. The Annotation application maintains association with the 3D model. As 
the 3D model is modified, the drawing will reflect the changes in 2D. 
2D Features. Just as you would expect in any other 2D CAD application, you can create 
dimensions, text, and 2D geometry using the Annotation application for CED. Add these 
features to your 3D view projections to complete your drawings. 
Bills of Material. A Bill of Material (BoM) can be generated in Annotation using multiple 
sources. You can also manually adjust the BoM in Annotation. BoM flags can be added to 
the drawing using DIN, ISO, or custom flag standards. 
Browsers. The Annotation application adds two new browsers to your interface. In 
Modeling, you only have the Structure browser. In Annotation, you’ve gained the Template 
browser and the Drawing browser. Similar to the Structure browser, both of your new 
browser are organized in a hierarchical fashion. The Templates browser organizes and ena-
bles the reuse of common objects. The Drawing browser organizes all drawing entities in 
session. 
DRAWING STRUCTURE 
 Within the drawing structure, owner-
ship falls to the parent. When a parent 
object is moved or deleted, the child is also 
moved or deleted. Navigate from object to 
object by clicking on their icons in the 
Drawing Browser. The hierarchy of the 
drawing structure looks like this: 
 
Drawing 
 Sheets 
 Frame 
 Sketch 
 Geometry of title block 
 Text of title block 
 Views 
 Dimensions 
 Text 
 Additional geometry 
 
VIEW SYNCHRONIZATION 
 View synchroniza-
tion is color coded. 
Dark Blue indicates that 
a view is totally up-to-
date. Cyan shows when 
a view is not updated, 
but the model is cur-
rently loaded in the 
Modeling application. 
Red tells you when the 
view cannot be updated because its associ-
ated model isn’t in memory. 
NOTE: When you click New Session in Annotation, it only clears the session 
within Annotation. To clear Annotation and Modeling, you’ll need to switch 
to the Modeling app and start a New Session as well. 
NOTE: Drawing-Model associativity is 
dictated by the views in the drawing. 
TEMPLATE BROWSER 
Templates allow you to reuse common 
text, sketches, and symbols. When added 
to a drawing, symbol templates can allow 
you to specify new values for named param-
eters. The “Smart” fields are filled-in as 
needed. The templates are viewed in your 
Template browser which became a new tab 
in your Structure Browser with the Annota-
tion Application. 
 Standard templates include GD&T 
Datum and Tolerance, Surface symbols, and 
Welding symbols. To add a Template to a 
drawing, simply double left-click the Tem-
plate from your template browser and fill-in 
the dialogue box for parameters and place-
ment. New user-defined Templates can be 
created and added to the Template browser 
as needed. 
 Define text and symbol can be found 
in the More dropdown of the Annotation 
group of the Annotation tab. Define sketch 
can be found under the Insert tab in the 
Sketch group. 
 To define a text or sketch template, 
use the appropriate type, enter a unique 
name, select a category from the dropdown 
list or create a new category, click the 
thumbnail checkbox to create a thumbnail, 
fill-in any other required boxes, and com-
plete the operation. 
 To defined new symbol templates, 
start with one that was defined from the 
standard templates. It can then be added 
to your templates itself to create anew tem-
plate; preserving your dialogue box settings 
for future use. 
QUICK REFERENCE GUIDE 
 28 
 
STARTING A DRAWING 
Start a drawing from the New Drawing command located under the An-
notation tab in the Setup group. You can not create any other annotation 
features until you create a drawing. You can only have one drawing loaded 
at a time, but each drawing can have multiple sheets. Take care to save 
your current drawing before opening another or start-
ing a new one. New Drawing creates a drawing and 
a sheet object in the Drawing Browser and then the 
dialogue box appears. 
The dialogue offers you three Modes of opera-
tion. 2D Process is the default and typical method. 
It will assume you want to take your 3D model and 
create 2D documentation from it. The 3D Process is 
all about creating 2D documentation from 3D doc-
uplanes. The third and final mode is No Model. It 
assumed there will be no 3D model association. You 
can always add it later. 
The dialogue that’s common to all three modes 
is Number, Sheet Frame, and Scale (Auto). Number 
represents the Sheet number. What do you want to 
call your sheet? It doesn’t need to be numeric and 
will accept alphanumeric characters, underscores, 
and spaces. It defaults to your model name. Select 
a sheet frame or None from the dropdown list to select a frame for your drawing.. Default 
options range from A0-4 to WM-E. The Scale (Auto) attempts to choose the correct scale 
based on the 3D model and the sheet frame chosen as you add views to the sheet frame in 
an attempt to make them all fit. You can choose a scale from the dropdown or specify one 
manually. You can always modify the individual view scale afterwards if necessary. If you 
click Add Views or simply complete the command, you’ll be immediately moved over into the 
New Std View command dialogue. 
Once you’ve created your drawing and initial sheet, you can create new 
sheets with the New Sheet command. You’ll be asked for the sheet Number, 
Sheet Frame, and Scale. Much as you were in the New Drawing dialogue. 
This dialogue doesn’t not automatically throw you into the New Std View com-
mand dialogue, though. You’re free to create new views or annotations as 
needed. 
DRAWING VIEWS 
 CED can generate several types 
of views. Use the New Std View com-
mand on your Annotation tab. The 
command dialogue box breaks your options 
down into different view categories. 
Orthogonal View. Orthogonal views 
refer to the common “Front”, “Top”, and 
“Right” viewing convention. Technically, 
views are orthogonal if they’re perpendicular 
to each other. So, to-
gether these three views 
form an orthogonal rep-
resentation of a part or 
assembly. 
Isometric. An iso-
metric view of an object 
is defined as viewing it in 
such a way that the an-
gles between the projec-
tion of the 3 axes are all 
the same (120°). Ob-
jects drawn with isomet-
ric projection do not ap-
pear larger or smaller as 
they extend from the 
viewer. 
General. Describes 
a view that ascribes to 
no specific convention. 
Choose a direction in the 
viewport and use the 
right-click menu to as-
sign the view. 
 
 
ANNOTATIONS: ANNOTATION APPLICATION 
Annotations 
 Profiles refer to a collection of 
settings that give you an optimal com-
bination of accuracy and performance. 
For example, you may want to use a 
Large Assembly profile for assemblies 
with over 500 parts. If so, the views update 
faster and small parts and tiny circles are 
automatically removed. Available profiles 
are Single Part, Small Assy, Medium Assy, 
Large Assy, Photo-Realistic, Shaded Only, 
Shaded+Geometry, and NC. 
Once your 
views are creat-
ed, you can 
adjust how the 
graphic data is 
updated by each view individ-
ually. Use your View Proper-
ties to adjust the Calc Mode. 
You can choose from Classic, 
Classic+Shaded, Graphics, 
Graphic+Shaded, and Shad-
ed update modes. Classic is 
the traditional dimensioned 
method. Graphics is better 
for larger models. Shaded 
best with renders that don’t 
geometry to be dimensioned. 
 Just below the Calc 
Mode, you’ll see Econofast. 
Econofast uses occlusion 
culling to give you a very fast 
and efficient view update, but 
requires an OpenGL-based 
graphics card. If you don’t 
have a compatible video 
card, the option will be 
grayed out. 
NOTE: All ME10 and Creo Elements/Direct Drafting drawings can be 
imported and re-associated with their models 
QUICK REFERENCE GUIDE 
 29 
 ANNOTATIONS: ANNOTATION APPLICATION 
Annotations 
PLACING VIEWS 
The New Std View dialogue box starts off with the 
owner of the view, and the orientation of the view. What 
this means is that CED can’t generate a view for you 
unless it understands the relative orientation of your part 
or assembly. The command chooses some defaults for 
you to make things easier, but understanding these re-
quirements can avoid a lot of frustration when working 
with more complex parts. 
Use the Front Dir or Up Dir options to open a 3D 
viewer that will present your part or assembly. You can then spin the model(s) around and 
use the 3D CoPilot widget to choose a front or up direction. These directions act as the 
references for all other view options in the dialogue box. You can also change the scale as 
needed. Scale is a ratio describing the relative size of your part or assembly on the drawing. 
A scale of 5:1 would indicate that every 5 units of measure in the drawing represented only 
1 on the part. Meaning that the drawing is five times larger than actual size. 1:1 being 
actual size. (Drawing : Part/Assy) 
At any point during the view definition where you have at least one type of view defined, 
you can click a point on your drawing to define placement. If you’re not happy with the 
placement, use Reposition Views to make updates until you are satisfied. Up until you com-
plete the view definition, you can add, remove, or reposition views as many times as you’d 
like. 
Your views will show-up as a hatched box on your drawing until you complete your view 
creation dialogue box. Once you’re done creating the views, you will not get the same dia-
logue box to edit the views you created. 
 After you’ve placed your views, you can use the Move View command to 
reposition, or simply click on the view border twice. The first click will bring up a 
mini toolbar in case you want to access some other view command. From there 
you can right-click for a contextual menu or click again. The second click acti-
vates Move View. 
CREATE DEPENDENT VIEWS 
Under the Annotation tab in the Setup 
group, you’ll see the Dep View drop-down. 
Each command has its 
own dialogue box. As you 
use a command you’ll no-
tice that the icon for the 
Dep View drop-down 
changes. You can quickly 
repeat the last command. 
The dependent view will show-up in 
the browsers underneath its parent. 
OUTLINE VIEWS 
If you want to conserve some time and 
don’t need the interior detail of a view, 
change the “Calculate Outline Only” property 
on your view. It will leave your view with 
nothing but the outline of whatever part or 
assembly was within. View Properties > 
Visibility > Calculate. 
 
 
UPDATING VIEWS 
You can Move and Scale a drawing view. 
You can also change a few options on de-
pendent views, but you can not change view 
type. The views are actually created in Creo 
Elements/Direct Modeling. 
The Annota-
tion application has the position on paper, 
scale, and such, but the Model contains the 
actual view. The two must work together to 
complete a drawing. 
To keep them working together, use 
Update View. This command will check the 
validity of your 3D model references and 
recreate your 2D projections if there’s been 
an update. 
Updated view geometry will change color 
according to the status of the 2D and 3Dgeometry. To see the colors, change Viewport 
Show Setting Upd Color. 
 
Unchanged Geometry = Magenta 
Changed Geometry = Yellow 
New Geometry = Cyan 
Changed 3D Documentation = Orange 
Transferred 2D Elements = Green 
Updated 2D Elements = Blue NOTE: Choose a Configuration 
from the view dialogue box or 
edit the view properties to 
display a Configuration rather 
than the assembled position. 
BEST PRACTICE: Always save your model after 
making Annotation changes and updates. Not 
just the drawing. Even if you don’t think that any-
thing in the model was changed. This prevents 
accidental inconsistencies between the two. 
QUICK REFERENCE GUIDE 
 30 
 ANNOTATIONS: ANNOTATION APPLICATION 
Annotations 
your selection. There are a series of Mod 
Position commands 
available in the same 
command group if 
you plan on moving 
more than the dimen-
sion. 
Single. Typical 
distance dimension 
from one point to another. 
Datum Long. A series of 
single dimensions attached to a 
datum on one end. 
Datum Short. Same as Datum Long 
except there’s no extension line on the 
datum. 
Chain. A stacked series of single di-
mensions where you have one occurring 
after the other in turn. 
Coordinate. A series of dimension 
lines in the X or Y direction based off of a 
single reference point. 
Chamfer. Dimensional call-out at-
tached to chamfer geometry. 
Sym Single. Same as a Single dimen-
sion but attached to a symmetry line. 
Sym Long. Same as a Symmetry Sin-
gle, but will automatically position subse-
quent dimensions relative to the first one. 
Aside from Linear dimensions, you also 
have Circular and Angular dimensions to 
choose from. 
Tangential. Dimensions 
a circle in tangential mode. 
Would be used for the length 
of a slot or distance between 
a point and a tangent point 
on a non-linear edge. 
Arc. Specify the actual linear length and 
actual angle of an arc. 
Angle. Measured in a clockwise direc-
tion. Switch between your selected angle, 
adjacent +, Opposite, and adjacent – by 
right-clicking during the dimension creation. 
DIMENSIONAL STANDARDS 
ASME/ANSI. American Society of Me-
chanical Engineers standards adopted from 
the American National Standards Institute. 
DIN. Deutsches Institut fur Normung. 
German institute for standardization. Mem-
ber of ISO. 
ISO. International Organization for 
Standardization is composed of representa-
tives from various national standards organ-
izations. 
JIS. Japanese Industrial Standards pro-
vided by the Japanese Industrial Standards 
committee and published through the Japa-
nese Standards Association. 
Custom. You can also create custom 
dimension standards to suit your needs. 
ANNOTATION 
Annotation is mainly about placing your 
2D features along with your projected views 
to complete the full representation of your 
3D objects for the purposes of illustration 
and/or manufacture. To that end, Creo 
Elements/Direct provides several tools for 
annotating your views. 
DIMENSIONS 
Each dimension 
has a type, attach-
ment, unit of measure, 
and adheres to one of 
four dimension stand-
ards. (or a custom 
standard) 
 Dimension com-
mands are found on 
the Annotation tab in the Annotate com-
mand group. Relocate a dimension the 
same way you would a View. Left-click the 
dimension twice. First click brings-up a mini 
toolbar and a right-click from that point will 
show the contextual menu where you can 
access dim properties. The second click 
initiates the Move Dim command against 
Chain Coordinate 
Chamfer 
Single 
Datum Long 
Diameter 
NOTE: Value, tolerance, format, text, and 
arrow adjustments can be made in the 
dimension properties dialogue box. 
ADDING TEXT 
Text can be added to drawings by man-
ually creating text, importing text from a file, 
or using a text template. 
Manually add text through 
the Text New command in the 
Annotation tab under the Anno-
tate group. The dialogue allows 
for changing style, angle, size, adjust point, 
ratio, slant, line space, font, fill, frame and 
color. Fill-in your text with the pop-up text 
editor and define a placement position. 
Import/Export text in the same Text 
New command using the pop-up text editor. 
Use the save and open options to grab or 
save *.txt, *.lsp, or *.rec files. 
Edit text with the Edit Text 
command through the mini 
toolbar, ribbon, or by right-
clicking on a selected text entity and select-
ing the command from the context menu. 
INSERTING OBJECTS 
You can insert pictures and OLE ob-
jects through the Insert tab of the Annota-
tion application. Pictures require a *.bmp, 
*.png, *.tif, *.jpg, *.jpeg, or *.tiff file type. 
You can also take a picture of a 3D or 2D 
viewport as your image using the Viewport 
dialogue box option. 
 You can embed objects from other 
applications into your drawing using an OLE 
object. For example, you could display a 
Microsoft Word or Excel document. 
QUICK REFERENCE GUIDE 
 31 
 ANNOTATIONS: ANNOTATION APPLICATION 
Annotations 
SKETCHING GEOMETRY 
Creo Elements/Direct Annotation Application comes with your typical 2D geometry cre-
ation tools under the Geometry tab; lines, rectangles, circles, splines, etc. It also includes 
the associated modification tools; copy, paste, rotate, mirror, stretch, trim, etc. 
Use these tools to create new 2D geometry in your drawing. The Annotation CoPilot will 
help guide your geometry creation. It provides incremental movement, size indication, snap 
lines, and 2D geometry snaps. 
Incremental movement can be adjusted using the Page Up or 
Page Down keys while creating geometry. The grid size will go from 3 
decimal places up to increments of 50,000 units in 26 steps. 
Size indication label shows the new element size or the modifica-
tion distance in a convenient X,Y format as you work. 
Snap lines appear when you move your cursor close enough to 
the catch point. By default, these snap lines are green. The catch 
points are added to your buffer by holding the cursor over a vertex 
for .5 seconds. (by default) A small plus sign will appear on the vertex. 
You can snap to start, end, and midpoints of lines, centers, and 2D geometry intersections. 
2D geometry snaps occur whenever a constraint 
requirement is met. You’ll see a green symbol if the 
constraint is snapping to snap lines or an orange symbol if it’s snapping to geometry. 
A Sketch acts as a container for 2D geometry. It can be found on the Insert tab under 
the Sketch group. To group geometry under a sketch, you can either create the geom-
etry first, and then use the Move command to change the owner of all your required 
geometry or you can create an empty sketch first and change owner of your geometry 
as you create it. You only need to set the owner dialogue of new geometry 
once. All subsequent geometry will default to the last owner. 
BOM TABLES 
Your Bill of Material (BoM) commands 
can be found under the Insert tab in the 
BoM command group. To place a BoM ta-
ble, you must first generate or import one. 
Use Scan Model to grab your BoM from an 
existing assembly. 
 Once you have BoM data, it can be 
accessed from the BoM Table command. 
Assign numbering using the BoM Numbering 
command. 
Draw your BoM onto the drawing using 
the Draw BoM command. In this dialogue, 
you assign the table layout and configure 
the growth direction, table range, and the 
table adjustment point. 
The table layout is what determines 
how the table is displayed and what data 
should be mapped. Default table layouts 
are Company, DIN, and ISO. Configure your 
own for specific columns, titles, or other 
requirements using the BoM Table Layout 
command. 
Place position flags using the Pos Flags 
command. Use dialogue option From 
Table to preserve your BoM Table number-
ing. Use flag layouts to govern the look of 
yourposition flags. Select the item from the 
BoM table, the geometry view, then flag 
position. 
PRINTING 
Printing is done in 
two ways depending on 
the type of printer chosen 
from the print dialogue 
box. Find the print dialogue in File Print. 
If you’re using a GDI printer, the raw 
print data is sent to the print spooler. The 
spooler then produces the final output. If 
using one of the generic printer types, the 
internal print drivers will generate the output 
and send it to a print file. 
Depending on your output device(s) 
configured on your machine, the Print Man-
ager may allow you to set several printer 
options in addition to those offered by Creo 
Elements/Direct Annotation. 
Typical print configurations are PDF, 
Clipboard, Laser (B&W), Laser (Color), Plot-
ter (Ink), and Plotter (Pen). You can choose 
from a large list of paper sizes, select an 
orientation, and even preview your settings 
directly on your Annotation viewport. 
3D SCREEN DUMPS 
If you want to capture your 3D viewport 
screen, you can create a High Resolution 
Print. Select the High Resolution Print from 
your print dialogue in the Creo Elements/
Direct Modeling Application. Alternately, 
right-click in your 3D viewport and select 
Viewport Properties. HR Print is one of the 
options and will bring up your printer set-
tings dialogue. You can also use this dia-
logue to Print the output to TIFF file 
rather that directly to a printer. 
NOTE: You can’t move a selection list of 2D geometry by selecting and double click-
ing. You must either group the geometry into a sketch or use the Move command. 
Tip: Try using the Grid Settings under File Settings Grid ... 
Perpendicular 
Vertical 
Horizontal 
Tangent 
Note: You can scan an existing BoM from 
the 3D Documentation Application or send 
the data from Model Manager BoM Editor. 
QUICK REFERENCE GUIDE 
 32 
 ANNOTATIONS: 3D DOCUMENTATION APPLICATION 
Annotations 
APPLICATION: 3D DOCUMENTATION 
The goal of the 3D Documentation Application is to communicate design ideas and 
thoughts in the 3D environment. It provides various capabilities to attach information to 
your design that may not have been easily captured by the geometry itself. For example, a 
specific manufacturing process. Activate the application by selecting File Modules and 
finding the Applications submenu. Put a check in the 3D Documentation check box. 
 Activating 3D Documentation creates three new tabs, one new envi-
ronment, and opens the template browser for your use. Annotate, 3D 
Documentation and Insert are your new tabs, but only the Annotate tab 
and template browser are accessible from the main Modeling application. 
The Annotate tab appears to the right of your existing tabs and is high-
lighted in blue. 
The new environment is accessed through the Applications tab. From there, you can 
switch back and forth between both environments. This is not a totally new session as with 
the Annotate Application, though. This is more like a modified Modeling environment. If you 
select New Session in either environment, it applies to both. They share the same memory 
space. In this 3D Documentation environment, the new Annotate tab becomes a command 
group under the 3D Documentation tab and you gain Setup and Display. Under the new 
Insert tab you gain BoM, Group, and Index. There are three other tabs available (Analysis, 
View, and Application), but these are standard fare from the Modeling application. 
 
 
 With 3D Documentation, you can create 3D dimensions, GD&T symbols, and notes. 
You can construct and implement Bills of Material (BoM) and attach position flags. Finally, 
you can create transfer your 3D dimensions and annotations over to the Annotation Applica-
tion. 
3D documentation has distinct advantages, like sharing im-
portant design information in the 3D environment with subsequent 
designers, indicating important dimensions, and describing specific 
manufacturing processes. Even so, you may not be able to share 
your 3D annotations with every manufacturer or simply want to com-
plete the documentation in the traditional 2D format. Your 3D 
documentation work is not lost. Using docuplanes, you can lever-
age your work and transfer it into the 2D Annotations Application. 
SETUP COMMAND GROUP 
A docuplane is similar to a workplane 
with only a few differences. A docuplane 
can be active at any time. A docuplane 
can not exist outside of a docuplane set. 
Also, docuplanes can not be saved individually. They are married to their own-
ing part or assembly. Finally, they are different in their purpose. A docuplane 
only exists to transfer 3D documentation into the 2D Annotation Application. 
First, create a docuplane set using New Set. This combo-command asks for the name 
and owner of the new set and also defines and underlying reference direction with the Front 
Dir and Up Dir options. As soon as you accept these options, the docuplane set is created 
and you’re thrown into the New Docuplane dialogue. The owning DP Set is already filled-in 
and you’re ready to choose a type and any other positional options for your new plane. You 
can create plane after plane from the same dialogue 
by clicking Next after each one. 
It’s important to understand how docuplanes 
are used to transfer data before you begin adding 
3D documentation to your design. If an annotation is not attached to a 
docuplane, it will not transfer. To attach an annotation to a docuplane, 
the annotation and docuplane must share an owner. Also, dimensions 
can not be transferred unless the docuplane it’s attached to is a valid 
display plane that is parallel to the measure direction of the dimension. 
Whenever you create an annotation, you’re given the option to attach it to a doc-
uplane. You can also modify an annotation for attachment after it’s been created or use 
the Gather command to assign free 3D annotations to docuplanes. To transfer these anno-
tations you must use the Transfer Docuplane from the Annotations Application and use 
Sync to DP to keep them up-to-date. 
In this relationship between docuplane and Annotation Application view, the doc-
uplane is the master. Dimension positions are not synchronized, but things like scale, up 
direction, normal, section line, detail border, name, or component list are all controlled by 
the docuplane. The synchronization will override any conflicting changes made in the An-
notations Application with docuplane values. If you need to alter these values more perma-
nently, make your changes in the docuplane to avoid having your changes overridden with 
the next sync. 
NOTE: Annotations are seen from either 
side of a docuplane. The labels flip as 
you rotate the view to remain readable. 
TIP: Matching Templates in the Template browser can make it easier to trans-
fer symbols between the 3D Documentation and Annotation Applications. 
QUICK REFERENCE GUIDE 
 33 
 ANNOTATIONS: 3D DOCUMENTATION APPLICATION 
Annotations 
ANNOTATE COMMAND GROUP 
Whether it be attached to a docuplane or free 
floating, an annotation can be created and modified 
through a series of commands in the Annotate com-
mand group. (The Annotate command group also 
exists in the Modeling application once the 3D Doc-
umentation application is activated.) 
Dimensions. Linear, circular, angular, coordinate, and datum 
long dimensions can be generated using the corresponding com-
mands. Coordinate dimensions form series of individual dimension 
lines based off of a single reference. Datum long dimensions are a 
series of single dimensions attached to a single datum on one end. 
The interface for attaching them to 3D geometry is a little different 
than what you’re used to in a 2D environment, but not by much. When you activate a di-
mension command, an elaborate dialogue box appears, but the actual dimension place-ment is intuitive. Click the element or start and end-points needed for your dimension oper-
ation, then place the dimension text. 
The 3D Note command will ask you for an element to attach a reference line. This 
referenced part becomes the owner of the note and the 3D Note a feature within it. For this 
reason, a 3D Note can only reference one feature of the model. They are generally used to 
specify manufacturing processes or specifications. 
 The dialogue will ask you for a docuplane or free placement. Then you can fill-in the 
actual note text using the pop-up text editor. This same editor will allow you to save and 
open text files. If you enter a Ref. URL, it will be displayed as a hyperlink in the feature re-
port’s URL column. If you click Ref. File, the browser options and allows you to link a file. 
Finally, you can choose the note type from Generic, Engineering, Manufacturing, or Inspec-
tion. These categories can be useful when filtering customer process features for reporting 
or highlighting purposes. 
Text objects are generally much more generic than the 3D Note. The dialogue box 
starts off asking for the text to be entered since reference lines are much less important to 
a text object. Enter or open your text as before, then add a primary reference. Optionally, 
add as many secondary references as you’d like. Define placement as docuplane or free, 
and place your text. 
Text generated in a dimension, 3D Note, or Text can be format-
ted using the Annotation 3D Properties command. You can change 
color, frame, display mode, anchor point, arrow type, size, and more. 
Access the Annotations 3D Properties command from the mini 
toolbar, the More dropdown, or right-click for the context menu. 
Modify your anno-
tations first with Orien-
tation (if needed) and 
then with Position. The 
Orientation command asks for Text Dir and 
Up Dir. Use any 3D references you’d like. 
Surprisingly, these two simple commands 
will quickly orient your annotations exactly 
as required. Once you have the annotation 
in the correct plane, use the Position com-
mand to move it In Plane (left and right, up 
and down, as if you were viewing it straight 
on a piece of paper directly in front of your 
eyes), or Thru Plane (closer or further away 
from you if viewed from the same orienta-
tion). Use Ref Position and Refline to 
change the reference line targets and ori-
entation. 
DISPLAY COMMAND GROUP 
Display has a few 
functions to help manage 
the visibility of your anno-
tations. Show will drop 
down to several com-
mands for docuplanes, 
groups, annotations, features, tolerances, 
and indexes. The Highlight drop down 
works for docuplanes, annotations, and 
features. HTML Reports can be generated 
to display a list of all custom features at-
tached to a model, assembly, workplane, 
WP set, or selection list. Create filters in 
the dialogue box before completing the 
command for cleaner output. 
MODIFY WITH DIMENIONS 
You may have noticed that the Move 
3D command has the option to use a dimen-
sion as a transformation reference. 
This will allow you to guide a transfor-
mation using a dimension, similar to how a 
parametric dimension might control geomet-
ric properties. The difference is that this 
relationship in CED is not exclusive. You’re 
fully capable of making more modifications 
with other references. Conversely, you can 
guide the transformation of any geometry 
using any dimensional reference. It’s not 
fully restricted to the geometry that’s been 
dimensioned. However, at least one ele-
ment must be directly to related to the di-
mensioned reference. 
This is very similar 
to behavior you might 
achieve using refer-
ence cones. With this 
method, though, 
there’s some sem-
blance of permanency. 
The dimensional refer-
ence remains to be 
used over and over if 
necessary. 
QUICK REFERENCE GUIDE 
 34 
 ANNOTATIONS: 3D DOCUMENTATION APPLICATION 
Annotations 
INSERT TAB 
The Insert tab contains command groups for the insertion and management of a Bill of 
Material (BoM) and an annotation Group. The BoM works similarly to the one in the Annota-
tion Application, but you’ll not be drawing the actual BoM table from here. This BoM group 
is geared towards placing flags only. A Group is an organizational tool for annotations. 
BOM COMMAND GROUP 
Use Collect to grab BoM data from your assembly or data management source. Collect 
a flat or multi-level BoM as needed. You can then use Table to see a pop-up dialogue de-
scribing your collected BoM, the new BoM table will start with empty position numbers. 
Placing flags will fill-in position numbers as you go. 
Placing flags with the New Pos 
Flag command will pop-up 
both the flag dialogue and the 
BoM table. You need to use 
them both, along with the 3D 
viewport for flag positioning. 
Double-click on a BoM table entry to fill in the BoM Entry box. The 
part highlights in the 3D viewport. Type a Number or go with the 
automatically assigned one. Choose docuplane or free. Optionally 
adjust your text orientation. Before you can complete the dialogue, 
you must choose a reference for the flag, which is some element on 
the geometry of the BoM Entry that your flag reference line will point to. An arrowhead will 
appear at the point you choose and a stretching reference line will allow you to place the 
label. The dialogue is set-up such that using the Next option can quickly take you through a 
BoM. 
Using Modify Pos Flag will take you to a very similar dialogue to the one used in crea-
tion, but the BoM table doesn’t appear and you’re not able to change the owner of the posi-
tion flag. You can, however, use Delete Pos Flag to remove ALL position flags from a given 
assembly. Simply use the command, click on the assembly, and confirm. If you need indi-
vidual deletion, just select a flag and hit your delete key. Use the annotation positioning 
and property commands to make adjustments to the display of your flag. 
GROUP COMMAND GROUP 
All annotation types can be contained 
in groups. Groups can also contain other 
groups. When selected, a group will return 
all children directly within it and all children 
of any subgroups. 
A New Fixed group can be quickly pro-
duced from a selection list. Simply define 
by clicking on the specific annotations 
you’re interested in grouping. Your selec-
tions can belong to any part or assembly 
owned by the group’s owner or by any sub-
assembly or subgroup thereof. 
You can create general or exclusive 
fixed groups. Within general fixed groups, a 
single annotation can belong to multiple 
groups. A general fixed group can be a 
parent or subgroup. Exclusive fixed groups 
can only be subgroups. They must have a 
parent group. Within exclusive fixed 
groups, an annotation can only belong to 
one group. That same annotation, howev-
er, can belong to several owners outside of 
the exclusive group hierarchy. 
A New Variable group is created with 
the intention of having the group update its 
own membership list. Membership is con-
trolled by a rule you generate from any 
number of annotation properties. 
To modify a group’s options or mem-
berships, right-click the group in your struc-
ture browser and choose the modify option. 
Use Show to highlight and traverse 
your annotation group hierarchies. You can 
also use Show to hide/show entire groups 
of annotations. 
Note: BoM data can be 
used by the Annotations 
Application using the 
Scan Model command. 
TEMPLATE BROWSER 
The Template browser in the 3D Docu-
mentation application is identical in behav-
ior to the one in the Annotation application 
with a few restrictions on the geometry al-
lowed in your symbols. You can not use 
splines, hatches, dimensions, symmetry 
lines, centerlines, construction lines, or 
points. Further, your elementscan not have 
a line size of zero. Text can not have a ratio 
of 1 and slant of 0. You must also have a 
frame on your text. 
Standard templates include GD&T Da-
tum and Tolerance, Surface symbols, and 
Welding symbols. The selection has been 
pruned to comply with the restrictions of 
being affixed to geometry in 3 dimensional 
space. To add a template, simply double 
left-click the template from your template 
browser or use the Create Symbol command 
and fill-in the dialogue box for parameters 
and placement. When added to a 
drawing, symbol templates can 
allow you to specify new values for 
named parameters. The “Smart” 
fields are filled-in as needed. 
New user-defined templates 
can be created and added to the 
template browser as needed 
using Define Template. 
Specify the default owner of 
any GD&T templates using GDT 
Owner. Any subsequently created 
GD&T templates will default to 
the specified owner. It’s located 
in the overflow menu More 
under the Annotate command 
group. 
QUICK REFERENCE GUIDE 
 35 
 MODEL MANAGER: INTRODUCTION 
Model Manager 
PRODUCT DATA MANAGEMENT SYSTEM 
Model Manager is the fully integrated Product Data Management (PDM) system for Creo Elements/Direct. Data management is extremely important when working with a large number 
of files and an extended design team. Manual file shares can be managed for a time, but quickly become more of a burden than a solution. Compare common data management concerns 
without and with a software solution in place. 
 Manually managed by a CAD administrator or by each design-
er. They create an elaborate system of folders to maintain 
data integrity. 
 There is usually nothing to prevent a designer from operating 
outside the convention other than doctrine. 
 Large numbers of files become increasingly difficult to manage 
as you approach the critical limit for hardware, networking, or 
have exhausted manual intervention options. 
 The IT department refuses to take ownership because of the 
overriding engineering knowledge required to decrypt the data 
structure and version control conventions. 
 Communicating data outside of the design team in a con-
sistent and efficient manner becomes virtually impossible. 
 CAD administrators usually develop a complex system of file 
naming to accommodate the need to maintain version history. 
 There is usually nothing to prevent a designer from operating 
outside the convention other than doctrine. 
 Versions become confused. Newer versions are overwritten 
due to lack of control. Older versions are duplicated across 
the elaborate data structure. 
 Permissions are usually ignored beyond the need to maintain 
a separation between administration and design. 
 In larger file share environments, departments are given own-
ership of file structure trees or segments in their entirety. 
Library data is copied across each segment. 
 Team or project based permission management is out of the 
question in most cases. 
 Data reuse is normally a file copy/paste exercise. Aside from 
the relationship corruptions, the difficulty is in knowing what’s 
available for reuse. Some teams print catalogs of categorized 
part images with file locations that are not kept up-to-date. 
 In larger file share environments, some have given-up on re-
use in general. The best they can manage is keeping the 
same designers on subsequent projects so they’re knowledge-
able enough to know what can be reused. 
WITHOUT A PDM SYSTEM 
 Product structure and file structure are maintained separately. 
What makes sense for the product is kept isolated from data 
management concerns. File structure become irrelevant to 
design and is maintained automatically. 
 File stores are still at the mercy of hardware limitations, but 
software solutions mitigate the impact of hardware and net-
working shortcomings on the design team. Hardware and 
networking issues are relegated to the IT department and data 
integrity is maintained automatically regardless of the file size 
or number of files within those limits. 
 Versions are maintained by the system. One file name is rep-
resentative of the latest version and all previous versions. 
Default interaction assumes the latest version, but version 
history is always available when needed. 
 Permissions can be left open or narrowed down to depart-
ment, project, team, or individual as necessary. You can even 
configure external access safely; Secure in the knowledge that 
your external visitors only have access to what they were given 
access to. 
 All objects in the system have a series of searchable attributes 
and notes associated with them that have been configured by 
your administration team to include everything your designers 
feel is important. Parts and assemblies have a special Save-
As type function that allows the user to reuse data without 
corrupting relationships. 
DATA STRUCTURE 
VOLUME OF DATA 
VERSION CONTROL 
PERMISSION CONTROL 
DATA REUSE 
CONCERNS WITH A PDM SYSTEM 
QUICK REFERENCE GUIDE 
 36 
 MODEL MANAGER: MODEL MANAGER BREAKDOWN 
Model Manager 
INTERFACE BREAKDOWN 
Model Manager comes in three pieces, generally speaking. First, your interface in Creo 
Elements/Direct Modeling is altered to accommodate Model Manger. Second, you get a 
brand new Workspace window for data management. Third, there’s a centralized database 
and a server application on your network that manage the storage and access of all CED 
hosted data. This guide will cover the first two pieces of Model Manager from the user per-
spective by describing, from a high level, the interface and capabilities. 
First, Creo Elements/Direct Modeling gains new right-click menus, file management 
menus, a new DB Attributes Browser, a new Model Manager tab and matching toolbar (View 
Toolbars), and most visibly gains bracket symbols [ ] to the right of each object in the 
Structure Browser. The Model Manager information is displayed in the Structure Browser as 
— Name [MajorRev.MinorRev] Status. 
 Second, the interface for the workspace window of Model Manager is very similar to 
Creo Elements/Direct. It has a quick access toolbar, ribbon UI, and a Details Panel on the 
left where the Structure Browser would be. The main viewport, now Information Panel, 
shows information specific to each tab of the Workspace Bar rather than your 3D models. 
The workspace acts as your window 
to data management outside of 
Creo Elements/Direct. 
 
DATA BREAKDOWN 
Model Manager stores all of your files 
in one large repository. Think of it as a 
software managed network drive without 
subfolders. The local workspace window 
provides a representation of the data sored 
in that central repository. That view is re-
freshed every 15 minutes (configurable). 
From Creo Elements/Direct, a refresh 
will show you a status message to the right 
of your model name. You’ll see things like 
New, Up-to-date, Locally modified, and Con-
flict. From the right-click menu you can 
choose to reload, save, or resolve data 
differences as needed. 
The default method for file storage is 
the 3D Data format provided by Creo Ele-
ments/Direct. It’s a very flexible format 
and offers direct access to part and assem-
bly files. There is only one data source per 
part or assembly. All iterations of the same 
part or assembly are simply references to 
the original. (This is contrary to package 
files where the same source data might be 
found in two different files) 
If you have an assembly with four 
unique parts in it, then the CED format will 
produce six files. 
 One assembly instance. *.sda 
 One assembly contents. *.sdac 
 Four part contents. *.sdpc 
ORGANIZATION BREAKDOWN 
The default method for data organiza-
tion is through the use of save/search/
load. All data resides in one place and you 
must fish for what you need through the 
use of search stringsand attribute hooks. 
<EnablePackets>true</EnablePackets> 
Beyond save/search/load, the primary 
method for organizing, controlling, and 
sharing your data is through the use of 
Packets. Your administrator must turn 
Packets on through the XML configuration 
file. 
 Packets are used to control and or-
ganize data within and send data outside 
of your PDM system. Once implemented, 
Packets change the typical workflow in 
Model Manager. 
 Nothing can be created, modified, or 
deleted unless it’s in a packet. Think of a 
packet as an envelope. Each user has their 
own envelope (or mailbox). You can’t open 
someone else's mail and they can’t open 
yours. However, for collaboration, you can 
send envelopes to whoever you need. 
<EnableProjects>false</EnableProjects> 
Projects and Folders offer a logical 
organization and permission control of data 
based on container ownership. These 
methods are provided for backwards com-
patibility only. They’re off by default. One 
major deficiency in Projects is that you can-
not assign roles or permissions directly to 
Folders. 
1) Quick Access Toolbar 
2) Ribbon UI 
3) Workspace Bar 
4) Quick Search 
5) Details Panel 
6) Info Panel 
 
 
Tip: Create new packets (envelopes) to organize 
your data into groups (mailboxes). Logically label 
them according to project, design phase, etc. 
BEST PRACTICE: Use the Refresh command 
to get the latest view of your data before 
making critical decisions with data that’s 
being manipulated by multiple designers. 
BEST PRACTICE: Model Manager is highly configurable and is rarely used for long without 
alteration. It excels at matching your preferences and processes. Plan on it. 
QUICK REFERENCE GUIDE 
 37 
 MODEL MANAGER: SEARCH AND LOAD 
Model Manager 
SEARCHING 
Search for information in your workspace window 
for Model Manager or the File Open From Model Man-
ager dialogue from CED. Use the quick search function 
or use the main search interface. Switch to the main 
search interface in Model Manger by clicking the Search tab in the Workspace Bar. 
 If you’re not using the Project, Folder, and Packet functionality, 
searching is your only method for finding data. There is no browsing 
other than any lists you’ve created; Recent List and Favorites. 
 The quick search includes the Name, Version, and Data Class of 
the objects in the database. Results are presented in the Information 
Panel below your Workspace Bar. 
 A full search can be executed from the Search tab in the Work-
space Bar. First, choose your data type. Then, you’ll see a set of at-
tributes associated with your data type. Your top 1000 search results 
(or fewer) will appear in the Information Panel. Search options, object 
preview, and details are available in the Detail Panel as you click 
through your results. 
 You can run similar searches from the File Open From Model 
Manager dialogue from Creo Elements/Direct. 
LOAD OPTIONS 
Single select or multi-select your mod-
els from the Recent List, Favorites, or Open 
dialogue. Load from your search results by 
right-click, double click, or ribbon UI. All 
roads lead to the same pop-up dialogue. 
 Having chosen your files, the Load 
Options Dialogue allows you to more specif-
ically decide which versions, structure 
members, and level of geometry you want 
to load. In most cases, you could likely 
forgo any further specification and simply 
click Load when this dialogue appears. The 
defaults will load your files at the highest 
revision with full geometry. 
Navigate the assembly structure by 
using the plus/minus icons on the left side 
of the table. 
Load Rules and Revision column. The 
Load rules are As Stored, Highest Revi-
sions, or Highest Released Revisions. De-
fault is Highest Revision. Make your rule 
selection to alter the entire list, but note 
that you can still make changes to the Revi-
sion column individually as needed. 
Use the Filter to scrub the list for Modi-
fiable Items, Non Modifiable Items, Full 
Geometry, Lightweight Model, or Partial 
(structure only). Notice that you can alter 
each individual item in the list by clicking 
the dropdown arrow next to the object icon. 
Masterdata is a meta-placeholder for 
all models, drawings, supporting docu-
ments, and BoM data for a specific manu-
factured instance. Masterdata is helpful 
when you have a part or assembly repre-
sented by more than one drawing or docu-
ment. It’s also helpful when you have one 
document that needs to be attached to 
many drawings. Picture a part that’s cast 
and molded in different colors with differ-
ent logos. When more than one master 
data exists you can select between them 
from the masterdata column. This will load 
the geometry and attach the information 
stored with the alternate masterdata. 
The Options submenu allows you to 
configure the way loading takes place. 
Your selections are saved and will carry 
from session to session. TIP: You can use ? as a single character and * as a general wildcard in searches. 
TIP: Save your complex searches so you can run them again later. 
QUICK REFERENCE GUIDE 
 38 
 MODEL MANAGER: SAVE AND CONFLICT RESOLUTION 
Model Manager 
SAVING DATA 
You can save data from several interface options. You 
can use the Model Manger tab inside Creo Elements/Direct 
(CED) ribbon. You can use the File Save to Model Manag-
er command from CED. Right-click your model in the Struc-
ture Browser for model manger save options. Use the model manger toolbar (View 
Toolbars). All roads lead to the same pop-up dialogue. 
The Save Options Dialogue allows you to 
specify save type, name, whether or not to 
create thumbnails, search, and filter. In most 
cases, you could likely forgo any further 
specification and simply click Save when this 
dialogue appears. Understanding your op-
tions will help you decide when that’s the 
case and when it’s not. 
The name value synchronizes with the 
Model Name attribute in Modeling. It 
can be set in the part properties, but if 
you don’t set it Model Manager will 
use the instance name. You’re given 
the opportunity to change the name in 
the save dialogue. This will be auto-
populated if using a number generator. 
Toggle the binocular icon to highlight or un-highlight table entries based on their status 
as modified items or new entries. Use the filter capability to scrub your table for modified 
items or new entries. 
There are four different Set Save Types. They will alter the versioning method across 
all entries in your table. Note that you can still make individual changes even after selecting 
a Set Save Type. Major Rev ALL Items will assume you want to go up one major revision for 
everything being saved regardless of its change status. Minor Rev MODIFIED Items (the 
Default) will add to your version history one minor revision level for every modified item in 
your save table. Major Rev MODIFIED Items will do the same but bump the major revision 
level. Overwrite MODIFIED Items doesn’t create a new revision. It overwrites the last revi-
sion with your new data. 
CONFLICTS 
Model Manager identifies potential problems before they happen. Without Model 
Manager these conflicts are usually left undetected until they become a major issue. The 
two types of conflicts are Name and SysID. 
A Name conflict occurs when someone attempts to save a model into Model Manager 
that has the same name, but different SysID of a model that already exists in Model Man-
ager. If it were a historical revision of the same part, it would have the same name and 
the same SysID. 
There are several ways to resolve a name conflict through the numerous methods to 
rename parts and assemblies. The Auto Number Generator can even help you avoid the 
issue altogether. If parts are set-up to use the Auto Number Generator, no duplicates 
occur.When they do occur, the name conflict resolution wizard can suggest a resolution 
for you. You can also use the wizard to enable a renaming rule to batch resolve a collec-
tion of similar conflicts. 
A SysID conflict occurs when you have a model in session from outside Model Manag-
er that has the same SysID and name as a model already stored in Model Manager. This 
usually happens when you load data from the hard drive while working with Model Manag-
er data. 
With a SysID conflict you can assign a new SysID to the object in session, replace your 
conflicting local data with Model Manager data, or replace Model Manager data with your 
local information. You should very rarely ever need to replace Model Manager data with 
your local information. If your session information is truly a newer revision of the existing 
Model Manager data, you should use the Make Version command rather than overwriting 
any data. 
Likewise, you should rarely use the Continue to Save option when you run into a con-
flict during a save operation. Investigate the conflict unless you’re absolutely certain of 
the issue and the impact of saving into Model Manager. 
NOTE: If you’ve configured the number generator, 
use the button to get the next number. Each 
subsequent click will increase the number by the 
configured value. 
ALERT: If you're using Packets, you can 
not overwrite unless the data is in a 
packet you own. 
NOTE: You can now save a full structure by 
saving the highest member. Lower members 
are automatically saved with the parent. 
BEST PRACTICE: SysID conflicts can also happen when storing package file data into 
Model Manager for the first time and when re-using data by making a copy and 
renaming it. 
 The Assign new SysID to local model command should be used any time new 
data is introduced into the system or copied from existing data. This will prevent 
corruptions and confusion down the road. 
QUICK REFERENCE GUIDE 
 39 
 MODEL MANAGER: BOMS, VERSIONING, AND INSEPERABLE OBJECTS 
Model Manager 
VERSIONING 
Versioning can be found in Creo Elements/Direct (CED) on 
the Structure tab under the Part & Assembly group. Companies 
don’t always model every component that they use internally. 
They’ll often send models out for revision, be contracted to work 
on a section of another design in progress, or themselves sub-
contract a section of a design to someone who doesn’t use Creo 
Elements/Direct. This situation can create major disturbances 
in the design process as each participant revises their section of 
the design. 
The main issue being resolved for CED has to do with the 
Model ID. Any time you load an imported model, it’s viewed 
as a new model and assigned a new Model ID. Therefore, 
you would need to manually re-integrate the new version into 
your design. As far as Model Manager is concerned, two dif-
ferent Model IDs means two different parts. 
Use Make Version to load and version the original part or assembly. This is where you 
might take a model from a vendor or contractor that’s done work on something you’ve 
already integrated into your design. 
INSEPARABLE OBJECTS 
Also in CED, you can Create Inseperable objects from the 
Inseperable dropdown under the Structure tab in the Part & As-
sembly group. Inseperable objects are created from assemblies 
that need to be represented in BoMs as a single part. For exam-
ple, you may have a welded assembly that is actually several 
parts but is purchased as and needs to be listed as a single part 
in the BoM. 
The Inseperable object will appear as a single part in subsequent BoM scans and ap-
pear in the Structure Browser with a distinctive red circle next to the assembly and part 
icons. See the Structure Browser icons in the appendix for examples. Reverse your chang-
es with the Separate command. 
The Bill of Material Editor in Model Manager can also flag objects as inseperable and 
reverse the change during the generation of a BoM report. The settings can be saved as a 
Configuration and reused as the BoM progresses through design. 
BILL OF MATERIAL EDITOR 
The Bill of Material (BoM) Editor is a separately licensed add-on module for Model Man-
ager. It can construct a BoM from the product structures housed in Model Manager. The 
use of the BoM Editor doesn’t require Creo Elements/Direct (CED). You can therefore rele-
gate BoM Editor responsibilities outside of design engineering. 
The BoM Editor uses masterdata information. Alternative masterdata entries can be 
used to build different BoMs so that multiple products can be made without needing to du-
plicate the design. To create masterdata, right click on your assembly and select Scan from 
the context menu. You can also find Scan under the Structure tab in the BoM group. 
Once you have masterdata to work with, use the BoM Editor command from the same 
right click context menu. You can also find the BoM Editor command under the Structure 
tab in the BoM group. From the BoM editor, you can add non-modeled parts like solder, 
paint, or lubricants. You can add spare and documentation items. You can also add pro-
cess specific tools or materials for manufacturing. 
The first time an item is added in this fashion, you will likely need to use the New Mas-
terdata command. An item that already has masterdata can be added with the Existing 
Masterdata command. Compare BoMs between versions or assemblies by using the Com-
pare BoMs command. 
Generate custom BoM reports from the Tools menu with the Generate Reports com-
mand. You can create flat, consolidated, and structured BoM reports. Include, exclude, 
show, and hide parts as necessary for your reports. You can explode an assembly structure 
using the Phantom option (uses the parts but not assembly structure) or define Inseparable 
assembly structures that should be treated as a single part rather than an assembly. Add 
or remove custom fields for the report like Effectivity or Options. Save all this back to your 
masterdata as a Con-
figuration so you don’t 
need to repeat the 
effort as things change. 
You can also use the 
Send To command to 
export a BoM to HTML, 
MS Excel, CSV, Annota-
tion, Drafting, and Mod-
eling. 
QUICK REFERENCE GUIDE 
 40 
 PLATFORM SUPPORT 
Appendix A: Support 
Operating System Windows 7 32-bit Editions: Ultimate, Enterprise, and Professional 
Windows 7 64-bit Editions: Ultimate, Enterprise, and Professional 
Windows Vista 32-bit Editions: Ultimate, Business, and Enterprise 
Windows Vista 64-bit Editions: Ultimate, Business, and Enterprise 
Windows XP Professional 
Windows XP Professional x64 
System Memory (RAM) Minimum: 1GB 
Recommended: 2GB or more 
Very large assemblies: 64-bit processor with 6GB or more 
CPU Intel Pentium (III, 4, M, D) 
Intel Xenon 
Intel Celeron 
Intel Core 
AMD Athelon 
AMD Opteron 
Note: Support for single and multi-core CPUs. 
Video Display Minimum: 1024x768 
Note: Available dual monitor support 
Workstations Available certified/supported workstations from different partners. 
http://www.ptc.com/partners/hardware/current/support.htm 
Optical Drive DVD 
Hard Disk Space During DVD Installation: 3GB 
Minimum: 2GB 
License Server At least one Create Elements/Direct License Server is required 
locally or within a network to host and maintain licenses for Creo 
Elements/Direct 18 products 
Virtual Machines Creo Elements/Direct Modeling 18.1 is not tested or certified on 
virtual machines such as Microsoft VirtualPC or VMware products. 
Creo Elements/Direct 18.1 
Operating System Windows 7 32-bit Editions: Ultimate, Enterprise, and Professional 
Windows Vista 32-bit Editions: Ultimate, Business, and Enterprise 
Windows XP Professional 
 
System Memory (RAM) Minimum: 512MB 
CPU Intel Pentium (III, 4, M, D) 
Intel Xenon 
Intel Celeron 
Intel Core 
AMD Athelon 
AMD Opteron 
Note: Support for single and multi-core CPUs.Optical Drive DVD 
Hard Disk Space During DVD Installation: 3GB 
Minimum: 300MB 
Model Manager 18.1 Client 
Operating System Windows Server 2008 R2 64-bit Edition 
Windows Server 2008 32-bit and 64-bit Editions of Standard and Enterprise 
Windows Server 2003 32-bit and 64-bit Editions of Standard and Enterprise 
Windows 7 32-bit and 64-bit Editions of Ultimate, Enterprise, and Professional 
Windows Vista 32-bit and 64-bit Editions of Ultimate, Enterprise, and Business 
Windows XP Professional 32-bit and 64-bit Editions 
System Memory (RAM) Minimum: 2GB (1-20 Creo Elements/Direct Model Manager clients) 
Optical Drive DVD 
Hard Disk Space During DVD Installation: 3GB 
Minimum: 18GB 
License Server At least one Creo Elements/Direct License Server is required locally or within a 
network to host and maintain licenses for Creo Elements/Direct 18 products. 
Virtual Machines Creo Elements/Direct Model Manager client and server are not tested or certi-
fied on virtual machines such as Microsoft VirtualPC or VMware products. 
Additional Information For specific, detailed system requirements please refer to 
http://www.ptc.com/partners/hardware/current/creo-elements-direct-
Model Manager 18.1 Server 
Platform support information is kept up-to-date by PTC at 
http://www.ptc.com/partners/hardware/current/support.htm 
QUICK REFERENCE GUIDE 
 41 
 TECHNICAL SUPPORT 
Appendix A: Support 
PTC TECHNICAL SUPPORT—PHONE 
PTC can be contacted via the phone for technical support and license management in 
local time zones and local languages. Support outside of the Monday-Friday business hours 
is provided only in English. If you’re current on maintenance and unless you made an addi-
tional investment in PTC support, you’re a Gold-level support customer. As such, you will 
receive phone support 24x5 during the workweek. GOLDplus customers get the addition of 
weekend support for critical issues. Platinum support customers receive continuous 24x7 
phone support. 
 United States and Canada Technical Support (800) 477-6435 
 United States and Canada Customer Care (877) ASK-4-PTC (877-275-4782) 
PTC TECHNICAL SUPPORT—WEB 
PTC provides a wealth of tools and information on the web. First, you need to have a 
PTC account. Once that’s in place, you may need to upgrade the account based on your 
customer information. PTC provides a knowledge base, case logger, case tracker, SPR 
Tracker, subscriptions, and more for your web based technical support needs. 
CREATING A PTC ACCOUNT 
In order to access PTC web support, 
users are required to create an account. 
This can be done by accessing the PTC 
website at www.ptc.com and clicking the 
“Login” link. From there click the “Create 
Basic Account” link and follow the dialogue. 
UPGRADING A PTC ACCOUNT 
Upgrade a basic account through the 
“Upgrade to a Customer Support Web Ac-
count” link and dialogue. Upgrading ena-
bles access to tools such as logging and 
tracking calls, software downloads, and 
searching the Knowledge Base. 
CASE LOGGER 
Create a new case to document a sin-
gle issue through the web or phone and a 
case number is generated for you. Subse-
quent emails, phone calls, file references, 
and all other records are tied to your case 
number. Find the Case Logger on the PTC 
support web site while logged-in. 
CASE TRACKER 
The Case Tracker allows customers to 
view the status of a case, see who’s as-
signed to the case, view history, and upload 
additional files. This is also where you’d 
escalate a case if necessary. Escalation will 
push the call up to a technical support man-
ager. 
 
SPR TRACKER 
A software performance report (SPR) 
documents an issue that requires a soft-
ware correction due to a bug or problem 
with the current software version and date-
code. An SPR can be generated if multiple 
call numbers or customers refer to a single 
issue. The SPR Tracker allows a customer 
to track the status and resolution of an 
SPR. 
 
PTC/USER SUBSCRIPTIONS 
PTC/User is a free, dedicated forum for 
the PTC user community. Share infor-
mation, tips and tricks, and issues with oth-
er users across the globe. It’s a great site to 
ask questions, receive answers, and discuss 
multiple PTC-related topics. 
 http://www.ptcuser.org 
 
COCREATE USER FORUM 
 The forum was originally sponsored by 
the CoCreate America’s User Group which 
has since dissolved. The main site hasn’t 
been updated since 2003, but the user 
forums are still active. They provide a his-
torical archive and current conversations. 
 http://www.cocreateusers.org/forum 
Case Logger 
PTC’s Support Website 
http://www.ptc.com/support/ 
NOTE: Signing up for a basic account will only give 
you access to basic functionality at PTC’s website. 
To gain access commensurate with your purchas-
es, it will be necessary to upgrade the account. 
BEST PRACTICE: The following are required in order 
to successfully upgrade a basic account. 
1. Customer Number 
2. Service Contract Number (SCN) or 
 Sales Order Number (SON) 
To find out how to obtain the customer number, 
SCN, and SON, refer to the Frequently Asked 
Questions page for Licensing on the PTC website 
by searching for the key word: PTC Order and 
License Support FAQ. 
QUICK REFERENCE GUIDE 
 42 
 CREO ELEMENTS/DIRECT SHORTCUTS 
Appendix B: Creo Elements/Direct Shortcuts 
KEYBOARD SHORTCUTS MOUSE BEHAVIOR 
VIEWPORT SHORTCUTS 
STRUCTURE BROWSER SHORTCUTS 
F1 Help on Current Context 
F2 Open Selection Menu 
F3 Toggle Global Axis 
F4 Toggle 3D Hidden Edges Visibility 
F5 Toggle 3D Geometry Visibility 
F6 Toggle 3D Shaded/Wireframe View 
F7 Toggle Workplane Borders Visibility 
F8 Toggle Local Workplane Axis Visibility 
F11 Toggle Full Screen for Current Viewport 
F12 Toggle Structure Browser 
Ctrl+Z Undo One 
Ctrl+Y Redo One 
Ctrl+Q Hide/Show Open Menus 
Ctrl+X Cut Selection to Clipboard 
Ctrl+C Copy Selection to Clipboard 
Ctrl+V Paste Selection Contents 
Ctrl+N New Session 
Ctrl+O Open Load Dialogue Window 
Ctrl+S Open Save Dialogue Window 
Ctrl+F Opens Search/Filter Dialogue from Structure Browser 
Left Click Select a single item 
Ctrl+Left Click Select multiple items 
Left Click and Hold Drag and drop 
Shift+Middle Click Expand or collapse select-
ed object 
Right-Click Display context-sensitive 
menu 
Double-Click Apply selection 
Right-Click  Apply Apply selection 
Space Open command specific mini toolbar 
Shift+Space Toggle command dialogue box 
Delete Delete selected 2D and 3D elements 
Tab Initiate or cycle to next selection method in 
sequence starting from initially highlighted face 
Shift+Tab Initiate or cycle to previous selection method in 
sequence starting from initially highlighted face 
(Boss/Pocket, Rib, Slot, Boss, and Pocket) 
Ctrl+Tab Activate probe selection 
Arrow keys Rotate view by 45° 
Shift+Arrow keys Rotate view by 3° 
Ctrl+Arrow keys Pan view 
R Relative measurement 
B Create a bend (arc) 
Z Undo the last 2D command 
Shift Suspend snapping 
I Ignore a snap 
L Toggle snap locking 
Delete Clear catch memory 
PgUp Increase adaptive grid size 
PgDn Decrease adaptive grid size 
Home Reset adaptive grid 
Shift+Ctrl Snap to center 
Left-Click Single select 
Start selection window (while dragging mouse) 
Selection list: Toggle selection list membership 
Middle-Click Ok/complete command (when mouse is still) 
Dynamic rotate (while dragging mouse) 
Right-Click Pop-up context sensitive menu (when mouse is still) 
Dynamic pan (while dragging mouse) 
Shift+Left-Click Select list start/resume 
Shift+Middle-Click Dynamic pan (while dragging mouse) 
Shift+Right-Click Pop-up menu with catch, select, and show options 
Ctrl+Left-Click Dynamic pan (while dragging mouse) 
Ctrl+Middle-Click Dynamic rotate (while dragging mouse) 
Ctrl+Right-Click Dynamic zoom (while dragging mouse) 
Alt+Middle-Click Over a face: New workplane on facethen start Line/Arc 
Shift+Alt+Middle-Click Over planar face: Move face by typed distance 
Shift+Alt+Left-Click Over planar face: Move face by From point and To point 
2D COPILOT SHORTCUTS 
Length Units 
um, mm, cm, m, km, uin, mil, 
inch, foot, yard mile 
Angle Units 
deg, rad, grd 
Angle Degrees to Decimal 
Degrees:Minutes:Seconds 
Math 
+, -, *, /, sin, cos, tan, asin, 
acos, atan, sqrt, exp, PI 
floor(n), ceil(n), ^ (power) 
DIALOGUE BOX 
CONVERSIONS 
Ctrl+H Hide elements 
Ctrl+U Unhide elements 
Shift+F4 Toggle tangent lines 
Shift+F5 Toggle sketched geometry 
Shift+F7 Toggle vertexes 
Shift+F10 Toggle update colors 
Shift+F11 Show template browser 
Shift+F12 Show drawing browser 
ANNOTATION APPLICATION KEYBOARD SHORTCUTS 
QUICK REFERENCE GUIDE 
 43 
 STRUCTURE BROWSER ICONS 
Appendix C: Structure Browser Icons 
Part 
Assembly 
Container 
Stock/finish relation 
Workplane 
Workplane set 
Face part 
Wire frame part (3D curve) 
Coordinate system 
3D view set of an Annotation drawing 
3D view of an Annotation drawing 
3D docuplane set 
3D docuplane 
Multi-section 
Part loaded with the lightweight option 
selected 
Configuration 
OBJECTS 
Modified 
Locked 
Multiple versions of a part loaded 
Shared part 
Shared assembly 
Selective instance 
Untouchable—due to open references 
the object cannot be modified 
Open references 
Partial assembly 
Partial part 
Partial container 
Partial workplane 
Partial workplane set 
Inseparable assembly 
Inseparable container 
Inseparable face part 
Inseparable part 
Inseparable stock/finish relation 
Inseparable wire part 
Inseparable workplane 
Inseparable workplane set 
Feature 
Part group 
Fixed or variable 3D annota-
tion group 
GD&T datum 
GD&T tolerance 
Applied taper feature 
Not applied taper feature 
Clipping feature 
Assembly which is a version of an original 
Part which is a version of an original 
Container which is a version of an original 
Workplane which is a version of an original 
Workplane set which is a version of an original 
Face part which is a version of an original 
Wire frame part which is a version of an original 
Partially loaded objects are displayed with the 
same icons shown in the partially loaded ob-
Drawing 
Sheet 
View updated using Econofast mode 
View updated using Graphics mode 
View — updated 
View—not updated 
View—error 
Flat view—updated 
Flat view—not updated 
Flat view—error 
OLE object 
Sketch 
Modified 
Frame 
Shared view—updated 
Shared view—not updated 
Shared view—error 
Section line 
Detail border 
Cutaway border 
Picture 
Stepped Hole 
Countersunk Partially Toleranced Through Hole 
Countersunk Through Hole 
Counterbored Through Hole 
Counterbored Through Hole with Chamfers 
Threaded Hole 
Partially Threaded Through Hole 
Partially Threaded Blind Hole 
Flat Blind Hole 
Countersunk Partially Toleranced Flat Blind Hole 
Countersunk Partially Toleranced Blind Hole 
Countersunk Flat Blind Hole 
Countersunk Blind Hole 
Blind Hole 
ANNOTATION 
STATUS 
INSEPARABLE 
FEATURES 
PARTIALLY LOADED 
MACHINING MODULE 
VERSIONS 
Up-to-date 
Out-of-date 
Invalid 
Partially loaded or lightweight 
subject or undefined 
CLASH ANALYSIS 
QUICK REFERENCE GUIDE 
 44 
 QUICK ACCESS TOOLBAR, RIBBON, PROMPT, AND USER INPUT LINE 
Appendix D: Interface Breakdown 
Quick Access Toolbar. Located in the upper left hand corner of the 
interface, it provides quick access to frequently-used commands. 
You can customize it by adding, removing and reordering commands 
(buttons and groups) to it. Right-click any command from the com-
mand search or ribbon UI to add them to the Quick Access Toolbar. 
The Ribbon UI is an interface style where a set of toolbars are placed 
on tabs in a tab bar at the top of the screen. Each tab in the ribbon 
contains icon commands that are organized into groups. This is also 
where you’ll see new colored tabs appear as modules and applica-
tions need them. 
 The ribbon UI provides an efficient layout for modeling 
commands. The most frequently used commands are displayed in 
large icons. Less common commands are displayed with smaller 
icons. Uncommonly used commands are grouped into submenus 
within each section of the ribbon. 
Prompt Bar. By default, displayed in the status bar on the bottom left corner of the interface. It provides general feedback, mes-
sages, and guidance. It can be removed from the Status Bar as its own entity using the Ribbon ViewToolbarsPrompt Bar. 
Closely Related Command Groups 
Functional Areas Divided Into Tabs 
Utilities Command Group Is 
commonly located on all but the 
View and Application tabs. It 
provides quick access to several 
frequently used utilities. 
Settings. Most command groups provide a settings button that provides quick ac-
cess to a dialogue for those system settings that are related to that command group. 
These same settings can also be accessed from the Settings menu located in the 
File tab. 
User Input Line. Several commands within Creo Elements/Direct 
will require keyboard input to complete without a dedicated 
dialogue box. Also, when drawing in 2D, you can enter coordi-
nates instead of clicking on the viewport. Use the U,V syntax 
with each coordinate separated by a comma. To specify several 
coordinates, separate each with a space. 
 Enter a command name to start that command. For exam-
ple, type “LINE” to start the Line command. You can also set 
and retrieve variable values using setf (S E T F) and the variable 
name. For example, “setf a 20” will make the variable “a” equal 
to the number “20”. Typing the variable name into the User 
Input Line is the same as typing its value. Note: String values 
must be contained in double quotes. 
QUICK REFERENCE GUIDE 
 45 
 STRUCTURE BROWSER, CATCH TOOLBAR, AND STATUS BAR 
Appendix D: Interface Breakdown 
Search and Filter icons will pop-up a dialogue 
used to find, filter, and display items from the 
Structure Browser based on your criteria. 
Status Bar is found on the lower right hand section of the main interface. It 
shows the alert history, current workplane, part, and settings for Catch and 
Units. Also shows pre-selection focus, quick viewport settings, and a "previous 
application" switch. Configurable on right-click. 
Structure Browser lists all currently loaded 3D objects and elements and shows their interrelationships through its hierarchal structure. You can control the display of 3D objects and ele-
ments using the check box next to each one. You can also expand and collapse the hierarchy as needed with the plus and minus symbols. The structure browser has a details display 
option toggled by the blue table icon located just below the Structure Browser tab icon. This alternate view will show a context sensitive list of properties. The browser area will also house 
new tabs like the Template Browser, Drawing Browser, and DB Attributes Browser as your active modules and applications that require a browser. It’s located on the left pane of the inter-
face but can be undocked and moved about. 
Catch Toolbar can be activated from the View tab or by clicking 
the Catch icon on the Status Bar. It controls the settings for your 2D 
and 3D snaps with three unique groups of settings. 
 Next Catch settings only apply to the very next caught entity. It 
returns to default settings after the next catch operation. 
 Default 2D and Default 3D refer to the default behavior in 2D 
mode and 3D mode for your next catch and every subsequent opera-
tion. Take care when making changes to these settings as they can 
have a drastic impact on the 2D and 3D modeling environments. 
Quick Viewport Settings. From left to 
right the viewport commands are Full 
Screen, Window, Last View, and Fit. 
QUICK REFERENCE GUIDE 
 46 
 FILE TAB 
Appendix D: Interface Breakdown 
File Tab is aunique tab providing the application’s most intrinsic commands. It pro-
vides load and save functionality, database access, print capability, and customiza-
tion. 
 New Session will wipe all objects from your current environment and start 
fresh. There is no Close option so a New Session is the best way to start anew other 
than closing and reopening the application. Open, Save, and Print work much like 
you’d expect from any other Windows based application with the exceptions of CAD 
specific nuances such as, opening a myriad of CAD data formats with extensible 
translation capabilities. Also, saving data out selectively to different file formats. 
The interaction with different data storage methods might also be a little different 
than Windows users may be use to, but the concept is the same — New, Open, Save, 
and Print. 
 Edit file will open the selected file in a separate text editor. The Modules sec-
tion is where you’ll make adjustments to which modules, applications, and interfaces 
are active in your environment. Some of these options will require licenses beyond 
the standard, but that’s clearly indicated in the dialogue. 
 Use Settings to tweak how your various functional areas look and operate while 
Customize will get into extensive toolbar, pop-up, and keyboard modifications. Op-
tions is where you make modifications to the Quick Access Toolbar, Ribbon UI, and 
your Command Mini Toolbars. 
 Finally, search for any command in the interface with your command finder at 
the bottom of the File tab. Results will be displayed in a list which replaces the rest 
of your File tab options while you’re searching. You can right-click results to add 
them to your Quick Access Toolbar or execute directly. Take note that the command 
finder search text looks in the command description as well as the command name. 
Toolbox is an empty menu 
that you can use to place 
your frequently-used com-
mands. You can drag this 
menu item to any toolbar 
or to the top menu bar 
itself in order to get faster 
access to the Toolbox 
buttons. 
QUICK REFERENCE GUIDE 
 47 
 MODELING, STRUCTURE, AND FEATURE TABS 
Appendix D: Interface Breakdown 
Modeling Tab contains most of your 2D and 3D object creation and manipulation tools. You’ll need to start with a workplane and a 2D profile to create 3D geometry, so those tools are available 
on this tab in the New and Draw groups. The 2D CoPilot will help streamline 2D profile creation. Tweak your 2D profile with commands from the Modify 2D group. Once you Pull some geometry, 
shape it with your intuitive 3D CoPilot and/or use the Model and Modify 3D commands. Round or Chamfer your edges or put your final Tapers in place with the Engineering group. 
Structure Tab. Through the use of different types of containers, the Structure Tab offers faster assembly manipulation, complex feature intelligence storage, helper object creation, and even a 
special container to store different assembly positions for your process drawings. Everything you would need to organize and prepare for assembly management and documentation. The Struc-
ture Tab also introduces the concepts of part and assembly sharing and instancing to capitalize on reuse. Your more advanced workplane commands are found here too. Some of the com-
mands in the Modeling tab and 3D Geometry tabs may require you to use the more advanced workplane tools found here. 
Feature Tab. The Feature tab organizes your parts. While Creo Elements/Direct is history free, it may become necessary, and it’s even recommended in some cases, to organize part history or 
design specific elements into containers for future reference. These commands allow you to group faces and other elements together into their own containers. The New Pattern command can 
only be executed against certain containers fashioned in this way. Part Group extends beyond the standard feature capability and can contain full parts, assemblies, and other containers. This 
tab is also where you’ll find the Machining operations if you’ve activated the Machining module. Finally, you have 3D dimensional annotations that can be added to your designs. These basic 
Annotation 3D commands are representative of the functionality you see extended in the 3D Documentation Application and can provide dimension features that can also be used as a modifica-
tion reference by the Move 3D command. 
QUICK REFERENCE GUIDE 
 48 
 3D GEOMETRY, ANALYSIS, AND VIEW TABS 
Appendix D: Interface Breakdown 
3D Geometry Tab contains your basic surfacing commands. You can add 3D curves, splines, and points. Use these to create and modify Face 
Parts for complex freeform surfaces. This is also where you’d gain access to the Wire Editor if you’ve activated the Parametrics Application. 
Analysis Tab provides Check Part to troubleshoot corrupt parts, Compare Parts to compare geometric and topologic information, and Clash/Interference reports and single evaluations. You’ll 
also find a comprehensive set of measurement tools here, some of which are repeated in the Utilities command group. Run color coded Draft analyses on your parts and Curve analyses on 
your 2D and 3D curves. This is also where you’d gain access to Angle and Surface analysis tools if you’ve activated the Surfacing Module. 
View Tab. Many of the view commands are built-in to the interface through the use of shortcut commands. Many, like isometric positioning and center selection, are exclusive to the Viewing 
group. Store custom camera views with Edit Camera and cycle through the list with the Next camera and Previous Camera commands. Create custom lighting, create, modify, and cycle through 
new viewports, and adjust model shading modes from the View tab. From here you can open or close current and legacy toolbars. The Clipping group provides invaluable visualization tools by 
adding methods to cut away model visibility with real-time editing capability. This is also where you’d gain access to the Render command if you have the Rendering module active. 
QUICK REFERENCE GUIDE 
 49 
 APPLICATIONS TAB 
Appendix D: Interface Breakdown 
Applications Tab comes fully loaded with all of the application icons available 
for Creo Elements/Direct Modeling. If the application is not active, the icon 
will be grayed out. You can activate/deactivate the applications, if you have 
access to the proper licenses, from the Modules dialogue box shown below. 
You can get to the Modules dialogue box from any of the three settings but-
tons under the Applications tab groups or from File Modules. 
 There’s also an Previous Application function that switches between your 
current application and the previously used application. The icon is located on 
the bottom right hand corner of your interface in the Status Bar. The Previous 
Application function is not a recognized command that can be found 
using the command search, but it can be added elsewhere in the 
interface using File Options. 
QUICK REFERENCE GUIDE 
 50 
 
Glossary 
Creo Elements/Direct (CED) PTC’s direct modeling me-
chanical CAD software. Purchased in 2007 as CoCreate. 
Re-branded to Creo Elements/Direct in 2010 as one of the 
three core elements that make-up the Creo software 
framework. 
CED Integration Kit A Creo Elements/Direct tools and doc-
umentation collection provided for the purposes of custom-
izing Creo Elements/Direct and programming add-on appli-
cations on top of Creo Elements/Direct. 
Creo Direct (CD) PTC’s new stand-alone Direct modeling 
software released under the Creo software framework in 
2011. 
Creo Parametric (CP) PTC’s mechanical CAD software re-
leased under the Creo software framework in 2011. His-
torically referred to as Pro/E. 
Creo Simulate (CP) PTC’s FEA software package released 
under the Creo software framework in 2011. Available as 
an extension to Creo Parametric or as a standalone appli-cation. Historically referred to as Mechanica. 
Creo View (CV) PTC’s viewing and interrogation software 
suite released under the Creo software framework in 
2011. Historically referred to as ProductView. 
Direct Modeling is the history free method of CAD where 
objects are manipulated based on existing geometry only; 
without conforming to a rigidly controlled design con-
straints system. (see Parametric) 
Drawing Browser Creo Elements/Direct Annotations inter-
face element located on the left pane. The drawing brows-
er provides a hierarchical display of object, container, and 
relationship information about drawing elements in ses-
sion memory. 
Drawlist In Creo Elements/Direct, refers to the list of ob-
jects and elements to be drawn in the 3D viewport. Its 
contents can be edited through the use of the check boxes 
in the Structure Browser. A separate drawlist is also stored 
with each Configuration feature. 
Drawing File (*.mi) Creo Elements/Direct Annotation 
standard file type for 2D drawings. The files maintain rela-
tionship information about the 3D models referred to by 
the associated 2D views in the drawing. The relationship is 
maintained on both ends and therefore both files must be 
saved after edits to maintain the relationship. 
 
Docuplanes Creo Elements/Direct 3D Documentation 
feature represented as a plane in the 3D viewport. Doc-
uplanes provide a position reference for annotations and a 
medium for the transfer of annotations from 3D to 2D. 
Dynamic Modeling Term originally coined by Hewlett Pack-
ard to describe their method for history free 3D CAD mod-
eling. Later referred to as Direct Modeling. 
Environment File (*.env) Creo Elements/Direct standard 
file type for the storage of user specific environmental da-
ta. The environment file contains information such as 
units, color of 2D geometry, and part and workplane ap-
pearance settings. 
Face Part A 3D part that is made-up of individual faces 
that do not form a solid body. In Creo Elements/Direct 
Modeling, a Face Part becomes a solid body automatically 
once the faces converge into a closed shell. 
Finite Element Analysis (FEA) The process of generating a 
computer model that then has theoretical stresses applied 
to it for the purposes of deriving the most likely physical 
results. 
Flexible Modeling Extension (FMX) Refers to a break-
through extension for Creo Parametric that allows a user to 
apply Direct modeling modification techniques to geometry 
in conjunction with the native parametric environment. 
Fluid UI PTC’s terminology for the interface of their Creo 
suite. Includes a Ribbon UI and Quick Access Toolbar simi-
2D Copilot Refers to the automated toolset which provides 
the functionality and feedback for creating all 2D geometry 
in Creo Elements/Direct Modeling. 
3D Copilot Refers to the 3D widgets and functionality pro-
vided by Creo Elements/Direct Modeling to facilitate the 
creation of all 3D elements. 
Access Control List (ACL) Describes a list of permissions 
for a given object or set of objects in a computer file sys-
tem. The ACL dictates who has access as well as what 
operations can be executed against an object. 
Bill of Material (BoM) In Creo Elements/Direct, a list of sub 
assemblies, parts, and the quantities of each as derived 
from a given assembly. A final production level BoM may 
include additional reference designators, attributes, and 
documentation. CED provides tools to derive, modify, and 
maintain production level BoMs. 
Bundle File (*.bdl) Creo Elements/Direct file type that 
ideally includes a 3D model and associated drawing that 
have been saved together from the Creo Elements/Direct 
Annotation application. 
Computer Aided Design (CAD) The use of computer sys-
tems to assist in the creation, modification, analysis, or 
optimization of a design. 
Camera Position In Creo Elements/Direct, refers to the 
position and orientation of the viewing perspective in a 3D 
viewport. 
Content File (*.sd*c) Creo Elements/Direct standard file 
type that contains the master workplane, part, or assembly 
properties, geometry, and topology information. 
Creo PTC’s newest line of CAD software applications fea-
turing a common data model, common user interface, and 
common application framework. The name Creo repre-
sents the software framework along with PTC’s develop-
ment path and vision for the future of CAD. 
GLOSSARY 
QUICK REFERENCE GUIDE 
 51 
 
Glossary 
ing design intent and enabling the easy modification of the 
design within those constraints. 
Parametric Technology Corporation (PTC) As one of the 
world’s largest and fastest-growing technology companies, 
PTC works with over 27,000 businesses worldwide in a 
wide array of manufacturing industries. They help manu-
facturers address the biggest business challenges they 
face. PTC provides software solutions for Product Lifecycle 
Management (PLM), Computer-Aided Design (CAD), Appli-
cation Lifecycle Management (ALM), Supply Chain Manage-
ment (SCM), and Service Lifecycle Management (SLM). 
Pro/Engineer (Pro/E) PTC’s parametric mechanical CAD 
software. Re-branded to Creo Elements/Pro in 2010 as 
one of the three core elements that make-up the Creo soft-
ware framework. Re-branded to Creo Parametric in 2011 
and released under the Creo framework. 
Product Data Management (PDM) Refers to the use of 
software to track and control file data related to product 
development. In CAD, a PDM also maintains the integrity 
of CAD specific file relationships, version control, and ac-
cess control. 
Product Lifecycle Management (PLM) Refers to the use of 
software to manage a single source of product information 
through its entire lifecycle; from inception to obsolescence. 
A PLM integrates people, data, process, and business sys-
tems to provide a software backbone for product develop-
ment companies. PLM systems typically have a wide range 
of functionality that’s uniquely configured to meet the indi-
vidual needs of each production environment they support. 
A PLM system is generally defined as providing multi-CAD 
product data management, varying degrees of embedded 
visualization, distributed collaboration capabilities, docu-
ment management, BoM management, configurable pro-
cess workflows, change management, and configuration 
management. Many PLM systems start with these capabil-
ities and scale well beyond them as needed. 
ProductView PTC’s viewing and interrogation software 
suite. Re-branded to Creo Elements/View in 2010 as one 
of the three core elements that make-up the Creo software 
framework. Re-branded to Creo View in 2011 and re-
leased under the Creo framework. 
Quick Access Toolbar Coined by Microsoft to refer to one 
of their user interface elements, the phrase refers to a 
customizable toolbar on the upper left corner of an applica-
tion that houses frequently used command icons and 
groups of the same. 
Ribbon UI Describes a major software interface element 
where virtually all toolbars and menus are placed in a se-
ries of narrow tabs that span the top of the window. Each 
tab in the ribbon contains command icons that are orga-
nized into functional groups and arranged according to 
frequency of use. These command groupings are fully con-
figurable in most environments. The Ribbon UI element is 
commonly recognized as part of Microsoft’s Fluent UI re-
leased with their Office suite. 
Session FIle (*.ses) Creo Elements/Direct file type meant 
for a fast and easy saving of all current data. They’re used 
for temporary storage of projects in progress typically out-
side of a PDM system. The session file saves all parts, 
assemblies, workplanes, workplane sets, and all environ-
ment settings. 
Structure Browser Creo Elements/Direct Modeling inter-
face element located on the left pane. The structure 
browser providesa hierarchical display of object, contain-
er, and relationship information for 3D elements in session 
memory. 
Template Browser Creo Elements/Direct interface element 
located on the left pane. The template browser provides 
clear display of stored templates of design symbols, regis-
tered sketches, and registered texts that can be added as 
3D and 2D annotation elements within the active session. 
lar to the Microsoft Office Fluent UI, unique mouse naviga-
tion, and a fluid look and feel to the overall colors, layout, 
and interface behaviors. 
Formations Goodie Creo Elements/Direct Modeling depre-
ciated add-on package provided to create assembly pro-
cess views. Replaced by Configuration features. 
GDI Printer Refers to a printer that has built-in support for 
the Windows Graphical Device Interface (GDI). 
GRANITE Refers to PTC’s feature-based interoperability, 
3D surface, and 3D solid modeling kernel. Specifically 
built to support a robust parametric modeling environment 
and data transitions between related software packages. 
HP Precision Engineering (HP PE) Hewlett-Packard’s suite 
of mechanical engineering centric CAD software. 
HP PE/ME30 Hewlett-Packard’s mechanical CAD package 
introduced in 1986 and transitioned away from in 1995. 
Instance File (*.sd*i) Creo Elements/Direct standard file 
type for a workplane, part, or assembly that works in con-
junction with a parent Content File. The Instance File con-
tains additional property and position data unique to the 
instance, but is dependent upon the Content File for base 
information. 
Package File (*.pkg) Creo Elements/Direct file type that 
potentially stores an entire design; assemblies, parts, and 
drawings. Typically used by solo engineers, design groups 
using file system storage, and designers who need to cre-
ate a complete design package to be sent to a partner. 
The package format is slower to update and comes with 
the intrinsic danger of creating multiple copies of data 
originally intended to be unique. 
Parametric Refers to the concept of a design being com-
pletely value driven; using dimensions and parameters to 
rigidly define and control the size and location of features 
and components. This is done for the purposes of captur-
GLOSSARY 
	Table of Contents
	Creo Elements/Direct Introduction
	Historical Overview
	Direct Modeling in Creo
	Creo Elements/Direct New Feature Highlights
	Modeling
	Interface Introduction
	Interface Summary
	Files, Ribbons, and Toolbars
	Right-Hand Rule
	Dialogue Boxes
	Calculator
	Workplanes
	Real and Construction Geometry
	Basic Modeling
	Catch, 2D CoPilot, Lock and Keyboard
	Modify 2D and Relative Measurement
	Putting it all Together
	Selecting Regions
	3D Copilot and Reference Cones
	Pull
	Selection
	Blends and Chamfers
	Moving and Pulling Faces
	Stretch Face, Edge, and Offset
	Taper Faces
	Cut, Copy, and Paste Faces
	Punch, Stamp, and Section
	Shell Imprint
	Boolean Operations
	Mirror, Scale, Align, and Merge
	Advanced Modeling
	Freeform Modeling
	Splines, 3D Curves and Points
	Projected Profiles
	3D Surfacing Tools
	Features and Patterns
	Modules
	Machining
	Surfacing
	Basic Sheets
	Assemblies
	Building Assembly Structures
	Containers
	Copy, Share, and Instancing
	Advanced Assemblies
	Clipping Planes
	Stock/Finish
	Coordinate Systems
	Configurations
	Explosions
	Clash Analysis
	Annotations
	Annotation Application
	Introduction
	Drawing Structure
	Template Browser
	Starting Drawing and Views
	Placing and Updating Views
	Adding Dimensions, Text, and Objects
	Sketing Geometry
	BoM Tables
	Printing
	3D Documentation Application
	Introduction
	Setup
	Annotate
	Display
	Modify with Dimensions
	BoM
	Group
	Template Browser
	Model Manager
	Introduction
	Model Manager Breakdown
	Search and Load
	Save
	Conflict Resolution
	Bill of Materials Editor
	Versions and Inseparable
	Appendix A - Support
	Platform Support
	Technical Support
	Appendix B - Shortcuts
	Creo Elements/Direct Shortcuts
	Appendix C - Structure Browser Icons
	Structure Browser Icons
	Appendix D - Interface Breakdown
	Quick Access Toolbar, Ribbon, Prompt, and User Input
	Structure Browser, Catch Toolbar, and Status Bar
	File Tab
	Modeling, Structure, and Feature Tabs
	3D Geometry, Analysis, and View Tabs
	Applications Tab
	Glossary
	Glossary
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