NX10 for Engineering Design

NX10 for Engineering Design
NX 10 for Engineering Design
By
Ming C. Leu
Amir Ghazanfari
Krishna Kolan
Department of Mechanical and Aerospace Engineering
Contents
FOREWORD ............................................................................................................1
CHAPTER 1 – INTRODUCTION ......................................................................... 2
1.1 Product Realization Process ..................................................................................................2
1.2 Brief History of CAD/CAM Development ...........................................................................3
1.3 Definition of CAD/CAM/CAE .............................................................................................5
1.3.1 Computer Aided Design – CAD .................................................................................. 5
1.3.2 Computer Aided Manufacturing – CAM ..................................................................... 5
1.3.3 Computer Aided Engineering – CAE........................................................................... 5
1.4. Scope of This Tutorial ..........................................................................................................6
CHAPTER 2 – GETTING STARTED .................................................................. 8
2.1 Starting an NX 10 Session and Opening Files ......................................................................8
2.1.1 Start an NX 10 Session................................................................................................. 8
2.1.2 Open a New File ........................................................................................................... 9
2.1.3 Open a Part File .......................................................................................................... 11
2.2 Printing, Saving and Closing Files ......................................................................................12
2.2.1 Print an NX 10 Image................................................................................................. 12
2.2.2 Save Part Files ............................................................................................................ 12
2.2.3 Close Part Files........................................................................................................... 13
2.2.4 Exit an NX 10 Session ............................................................................................... 14
2.3 NX 10 Interface ...................................................................................................................14
2.3.1 Mouse Functionality ................................................................................................... 14
2.3.2 NX 10 Gateway .......................................................................................................... 17
2.3.3 Geometry Selection .................................................................................................... 21
2.3.4 User Preferences ......................................................................................................... 22
2.3.5 Applications ............................................................................................................... 25
2.4 Layers ..................................................................................................................................26
2.4.1 Layer Control ............................................................................................................. 26
2.4.2 Commands in Layers .................................................................................................. 27
2.5 Coordinate Systems .............................................................................................................29
2.5.1 Absolute Coordinate System ...................................................................................... 29
2.5.2 Work Coordinate System ........................................................................................... 29
2.5.3 Moving the WCS ........................................................................................................ 29
2.6 Toolbars ..............................................................................................................................30
CHAPTER 3 – TWO DIMENSIONAL SKETCHING......................................33
3.1 Overview .............................................................................................................................33
3.2 Sketching Environment .......................................................................................................34
3.3 Sketch Curve Toolbar .........................................................................................................35
3.4 Constraints Toolbar .............................................................................................................37
3.5 Examples .............................................................................................................................40
3.5.1 Arbor Press Base ........................................................................................................ 40
3.5.2 Impeller Lower Casing ............................................................................................... 44
3.5.3 Impeller ...................................................................................................................... 48
CHAPTER 4 – THREE DIMENSIONAL MODELING ...................................50
4.1 Types of Features ................................................................................................................50
4.1.1 Primitives ................................................................................................................... 51
4.1.2 Reference Features ..................................................................................................... 51
4.1.3 Swept Features ........................................................................................................... 52
4.1.4 Remove Features ........................................................................................................ 53
4.1.5 Extract Features .......................................................................................................... 53
4.1.6 User-Defined features ................................................................................................ 54
4.2 Primitives ............................................................................................................................54
4.2.1 Model a Block ............................................................................................................ 54
4.2.2 Model a Shaft ............................................................................................................. 56
4.3 Reference Features ..............................................................................................................58
4.3.1 Datum Plane ............................................................................................................... 58
4.3.2 Datum Axis ................................................................................................................ 60
4.4 Swept Features ....................................................................................................................61
4.5 Remove Features .................................................................................................................65
4.5.1 General Hole .............................................................................................................. 66
4.5.2 Pocket ......................................................................................................................... 68
4.5.3 Slot ............................................................................................................................. 68
4.5.4 Groove ........................................................................................................................ 68
4.6 Feature Operations ..............................................................................................................69
4.6.1 Edge Blend ................................................................................................................. 69
4.6.2 Chamfer ...................................................................................................................... 69
4.6.3 Thread......................................................................................................................... 70
4.6.4 Trim Body .................................................................................................................. 71
4.6.5 Split Body................................................................................................................... 71
4.6.6 Mirror ......................................................................................................................... 71
4.6.7 Pattern......................................................................................................................... 72
4.6.8 Boolean Operations .................................................................................................... 73
4.6.9 Move........................................................................................................................... 73
4.7 Examples .............................................................................................................................75
4.7.1 Hexagonal Screw........................................................................................................ 75
4.7.2 Hexagonal Nut ............................................................................................................ 78
4.7.3 L-Bar .......................................................................................................................... 81
4.7.4 Rack ............................................................................................................................ 85
4.7.5 Impeller ...................................................................................................................... 89
4.8 Standard Parts Library.........................................................................................................92
4.9 Synchronous Technology ....................................................................................................93
4.10 Exercises ...........................................................................................................................96
4.10.1 Circular Base ............................................................................................................ 96
4.10.2 Impeller Upper Casing ............................................................................................. 96
4.10.3 Die-Cavity ................................................................................................................ 97
CHAPTER 5 – DRAFTING ..................................................................................99
5.1 Overview .............................................................................................................................99
5.2 Creating a Drafting............................................................................................................100
5.3 Dimensioning ....................................................................................................................105
5.4 Sectional View ..................................................................................................................108
5.5 Product and Manufacturing Information...........................................................................109
5.6 Example.............................................................................................................................112
5.7 Exercise .............................................................................................................................116
CHAPTER 6 – ASSEMBLY MODELING .......................................................117
6.1 Terminology ......................................................................................................................117
6.2 Assembling Approaches....................................................................................................118
6.2.1 Top-Down Approach................................................................................................ 118
6.2.2 Bottom-Up Approach ............................................................................................... 118
6.2.3 Mixing and Matching ............................................................................................... 119
6.3 Assembly Navigator ..........................................................................................................119
6.4 Mating Constraints ............................................................................................................120
6.5 Example.............................................................................................................................120
6.5.1 Starting an Assembly ............................................................................................... 121
6.5.2 Adding Components and Constraints ....................................................................... 124
6.5.3 Exploded View ......................................................................................................... 132
6.6 Exercise .............................................................................................................................135
CHAPTER 7 – FREEFORMING ......................................................................137
7.1 Overview ...........................................................................................................................137
7.1.1 Creating Freeform Features from Points .................................................................. 138
7.1.2 Creating Freeform Features from Section Strings .................................................... 138
7.1.3 Creating Freeform Features from Faces ................................................................... 139
7.2 FreeForm Feature Modeling .............................................................................................139
7.2.1 Modeling with Points ............................................................................................... 140
7.2.2 Modeling with a Point Cloud ................................................................................... 141
7.2.3 Modeling with Curves .............................................................................................. 143
7.2.4 Modeling with Curves and Faces ............................................................................. 144
7.3 Exercise .............................................................................................................................146
CHAPTER 8 – FINITE ELEMENT ANALYSIS .............................................147
8.1 Overview ...........................................................................................................................147
8.1.1 Element Shapes and Nodes ...................................................................................... 147
8.1.2 Solution Steps ........................................................................................................... 149
8.1.3 Simulation Navigator ............................................................................................... 150
8.2 Scenario Creation ..............................................................................................................150
8.3 Material Properties ............................................................................................................153
8.4 Meshing .............................................................................................................................155
8.5 Loads .................................................................................................................................156
8.6 Boundary Conditions ........................................................................................................157
8.7 Result and Simulation .......................................................................................................158
8.7.1 Solving the Scenario................................................................................................. 158
8.7.2 FEA Result ............................................................................................................... 159
8.7.3 Simulation and Animation ....................................................................................... 162
8.8 Exercise .............................................................................................................................164
CHAPTER 9 – MANUFACTURING ................................................................165
9.1 Getting Started ..................................................................................................................165
9.1.1 Creation of a Blank .................................................................................................. 165
9.1.2 Setting Machining Environment .............................................................................. 167
9.1.3 Operation Navigator ................................................................................................. 168
9.1.4 Machine Coordinate System (MCS) ........................................................................ 169
9.1.5 Geometry Definition ................................................................................................ 169
9.2 Creating Operation ............................................................................................................170
9.2.1 Creating a New Operation ........................................................................................ 170
9.2.2 Tool Creation and Selection ..................................................................................... 171
9.2.3 Tool Path Settings .................................................................................................... 174
9.2.4 Step Over and Scallop Height .................................................................................. 175
9.2.5 Depth Per Cut ........................................................................................................... 176
9.2.6 Cutting Parameters ................................................................................................... 176
9.2.7 Avoidance................................................................................................................. 177
9.2.8 Speeds and Feeds ..................................................................................................... 178
9.3 Program Generation and Verification ...............................................................................180
9.3.1 Generating Program ................................................................................................. 180
9.3.2 Tool Path Display ..................................................................................................... 180
9.3.3 Tool Path Simulation ................................................................................................ 181
9.3.4 Gouge Check ............................................................................................................ 183
9.4 Operation Methods ............................................................................................................184
9.4.1 Roughing .................................................................................................................. 184
9.4.2 Semi-Finishing ......................................................................................................... 184
9.4.3 Finishing Profile ....................................................................................................... 187
9.4.4 Finishing Contour Surface ....................................................................................... 191
9.4.5 Flooring .................................................................................................................... 195
9.5 Post Processing .................................................................................................................197
9.5.1 Creating CLSF.......................................................................................................... 198
9.5.2 Post Processing ......................................................................................................... 199
FOREWORD
NX is one of the world’s most advanced and tightly integrated CAD/CAM/CAE product
development solution. Spanning the entire range of product development, NX delivers immense
value to enterprises of all sizes. It simplifies complex product designs, thus speeding up the process
of introducing products to the market.
The NX software integrates knowledge-based principles, industrial design, geometric modeling,
advanced analysis, graphic simulation, and concurrent engineering. The software has powerful
hybrid modeling capabilities by integrating constraint-based feature modeling and explicit
geometric modeling. In addition to modeling standard geometry parts, it allows the user to design
complex free-form shapes such as airfoils and manifolds. It also merges solid and surface modeling
techniques into one powerful tool set.
This self-guiding tutorial provides a step-by-step approach for users to learn NX 10. It is intended
for those with no previous experience with NX. However, users of previous versions of NX may
also find this tutorial useful for them to learn the new user interfaces and functions. The user will
be guided from starting an NX 10 session to creating models and designs that have various
applications. Each chapter has components explained with the help of various dialog boxes and
screen images. These components are later used in the assembly modeling, machining and finite
element analysis. The files of components are also available online to download and use. We first
released the tutorial for Unigraphics 18 and later updated for NX 2 followed by the updates for
NX 3, NX 5, NX 7 and NX 9. This write-up further updates to NX 10.
Our previous efforts to prepare the NX self-guiding tutorial were funded by the National Science
Foundation’s Advanced Technological Education Program and by the Partners of the
Advancement of Collaborative Engineering Education (PACE) program.
If you have any questions or comments about this tutorial, please email Ming C. Leu at
[email protected] or Amir Ghazanfari at [email protected] The models and all the versions of the
tutorial are available at http://web.mst.edu/~mleu.
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CHAPTER 1 – INTRODUCTION
The modern manufacturing environment can be characterized by the paradigm of delivering
products of increasing variety, smaller batches and higher quality in the context of increasing
global competition. Industries cannot survive worldwide competition unless they introduce new
products with better quality, at lower costs and with shorter lead-time. There is intense
international competition and decreased availability of skilled labor. With dramatic changes in
computing power and wider availability of software tools for design and production, engineers are
now using Computer Aided Design (CAD), Computer Aided Manufacturing (CAM) and Computer
Aided Engineering (CAE) systems to automate their design and production processes. These
technologies are now used every day for sorts of different engineering tasks. Below is a brief
description of how CAD, CAM, and CAE technologies are being used during the product
realization process.
1.1 PRODUCT REALIZATION PROCESS
The product realization process can be roughly divided into two phases; design and manufacturing.
The design process starts with identification of new customer needs and design variables to be
improved, which are identified by the marketing personnel after getting feedback from the
customers. Once the relevant design information is gathered, design specifications are formulated.
A feasibility study is conducted with relevant design information and detailed design and analyses
are performed. The detailed design includes design conceptualization, prospective product
drawings, sketches and geometric modeling. Analysis includes stress analysis, interference
checking, kinematics analysis, mass property calculations and tolerance analysis, and design
optimization. The quality of the results obtained from these activities is directly related to the
quality of the analysis and the tools used for conducting the analysis.
The manufacturing process starts with the shop-floor activities beginning from production
planning, which uses the design process drawings and ends with the actual product. Process
planning includes activities like production planning, material procurement, and machine
selection. There are varied tasks like procurement of new tools, NC programming and quality
checks at various stages during the production process. Process planning includes planning for all
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the processes used in manufacturing of the product. Parts that pass the quality control inspections
are assembled functionally tested, packaged, labeled, and shipped to customers.
A diagram representing the Product Realization Process (Mastering CAD/CAM, by Ibrahim Zeid,
McGraw Hill, 2005) is shown below.
1.2 BRIEF HISTORY OF CAD/CAM DEVELOPMENT
The roots of current CAD/CAM technologies go back to the beginning of civilization when
engineers in ancient Egypt recognized graphics communication. Orthographic projection practiced
today was invented around the 1800s. The real development of CAD/CAM systems started in the
1950s. CAD/CAM went through four major phases of development in the last century. The 1950s
was known as the era of interactive computer graphics. MIT’s Servo Mechanisms Laboratory
demonstrated the concept of numerical control (NC) on a three-axis milling machine. Development
in this era was slowed down by the shortcomings of computers at the time. During the late 1950s
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the development of Automatically Programmed Tools (APT) began and General Motors explored
the potential of interactive graphics.
The 1960s was the most critical research period for interactive computer graphics. Ivan Sutherland
developed a sketchpad system, which demonstrated the possibility of creating drawings and
altercations of objects interactively on a cathode ray tube (CRT). The term CAD started to appear
with the word ‘design’ extending beyond basic drafting concepts. General Motors announced their
DAC-1 system and Bell Technologies introduced the GRAPHIC 1 remote display system.
During the 1970s, the research efforts of the previous decade in computer graphics had begun to
be fruitful, and potential of interactive computer graphics in improving productivity was realized
by industry, government and academia. The 1970s is characterized as the golden era for computer
drafting and the beginning of ad hoc instrumental design applications. National Computer
Graphics Association (NCGA) was formed and Initial Graphics Exchange Specification (IGES)
was initiated.
In the 1980s, new theories and algorithms evolved and integration of various elements of design
and manufacturing was developed. The major research and development focus was to expand
CAD/CAM systems beyond three-dimensional geometric designs and provide more engineering
applications.
The present day CAD/CAM development focuses on efficient and fast integration and automation
of various elements of design and manufacturing along with the development of new algorithms.
There are many commercial CAD/CAM packages available for direct usages that are user-friendly
and very proficient.
Below are some of the commercial packages in the present market.
•
Solid Edge, AutoCAD and Mechanical Desktop are some low-end CAD software systems,
which are mainly used for 2D modeling and drawing.
•
NX, Pro-E, CATIA and I-DEAS are high-end modeling and designing software systems
that are costlier but more powerful. These software systems also have computer aided
manufacturing and engineering analysis capabilities.
•
ANSYS, ABAQUS, NASTRAN, and COMSOL are packages mainly used for analysis of
structures and fluids. Different software are used for different proposes.
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•
Geomagic and CollabCAD are some of the systems that focus on collaborative design,
enabling multiple users of the software to collaborate on computer-aided design over the
Internet.
1.3 DEFINITION OF CAD/CAM/CAE
Following are the definitions of some of the terms used in this tutorial.
1.3.1 Computer Aided Design – CAD
CAD is technology concerned with using computer systems to assist in the creation, modification,
analysis, and optimization of a design. Any computer program that embodies computer graphics
and an application program facilitating engineering functions in design process can be classified
as CAD software.
The most basic role of CAD is to define the geometry of design – a mechanical part, a product
assembly, an architectural structure, an electronic circuit, a building layout, etc. The greatest
benefits of CAD systems are that they can save considerable time and reduce errors caused by
otherwise having to redefine the geometry of the design from scratch every time it is needed.
1.3.2 Computer Aided Manufacturing – CAM
CAM technology involves computer systems that plan, manage, and control the manufacturing
operations through computer interface with the plant’s production resources.
One of the most important areas of CAM is numerical control (NC). This is the technique of using
programmed instructions to control a machine tool, which cuts, mills, grinds, punches or turns raw
stock into a finished part. Another significant CAM function is in the programming of robots.
Process planning is also a target of computer automation.
1.3.3 Computer Aided Engineering – CAE
CAE technology uses a computer system to analyze the functions of a CAD-created product,
allowing designers to simulate and study how the product will behave so that the design can be
refined and optimized.
CAE tools are available for a number of different types of analyses. For example, kinematic
analysis programs can be used to determine motion paths and linkage velocities in mechanisms.
Dynamic analysis programs can be used to determine loads and displacements in complex
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assemblies such as automobiles. One of the most popular methods of analyses is using a Finite
Element Method (FEM). This approach can be used to determine stress, deformation, heat transfer,
magnetic field distribution, fluid flow, and other continuous field problems that are often too tough
to solve with any other approach.
1.4. SCOPE OF THIS TUTORIAL
This tutorial is written for students and engineers who are interested in learning how to use NX 10
for designing mechanical components and assemblies. Learning to use this software will also be
valuable for learning how to use other CAD systems such as PRO-E and CATIA.
This tutorial provides a step-by-step approach for learning NX 10.
Chapter 2 includes the NX 10 essentials from starting a session to getting familiar with the NX
10 layout by practicing basic functions such as Print, Save, and Exit. It also gives a brief description
of the Coordinate System, Layers, various toolboxes and other important commands, which will
be used in later chapters.
Chapter 3 presents the concept of sketching. It describes how to create sketches and to give
geometric and dimensional constraints. This chapter is very important since present-day
components are very complex in geometry and difficult to model with only basic features.
The actual designing and modeling of parts begins with chapter 4. It describes different features
such as reference features, swept features and primitive features and how these features are used
to create designs. Various kinds of feature operations are performed on features.
You will learn how to create a drawing from a part model in chapter 5. In this chapter, we
demonstrate how to create a drawing by adding views, dimensioning the part drawings, and
modifying various attributes in the drawing such as text size, arrow size and tolerance.
Chapter 6 teaches the concepts of Assembly Modeling and its terminologies. It describes TopDown modeling and Bottom-Up modeling. We will use Bottom-Up modeling to assemble
components into a product.
Chapter 7 introduces free-form modeling. The method of modeling curves and smooth surfaces
will be demonstrated.
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Chapter 8 is capsulated into a brief introduction to Design Simulations available in NX 10 for the
Finite Element Analysis.
Chapter 9 will be a real-time experience of implementing a designed model into a manufacturing
environment for machining. This chapter deals with generation, verification and simulation of Tool
Path to create CNC (Computer Numerical Codes) to produce the designed parts from multiple axes
and even advanced CNC machines.
The examples and exercise problems used in each chapter are so designed that they will be finally
assembled in the chapter. Due to this distinctive feature, you should save all the models that you
have generated in each chapter.
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CHAPTER 2 – GETTING STARTED
We begin with starting of an NX 10 session. This chapter will provide the basics required to use
any CAD/CAM package. You will learn the preliminary steps to start, to understand and to use the
NX 10 package for modeling, drafting, etc. It contains five sub-sections a) Opening an NX 10
session, b) Printing, saving, and closing part files, c) getting acquainted with the NX 10 user
interface d) Using layers and e) Understanding important commands and dialogs.
2.1 STARTING AN NX 10 SESSION AND OPENING FILES
2.1.1 Start an NX 10 Session
 From the Windows desktop screen, click on Start →All Programs →Siemens NX 10 →
NX 10
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The main NX 10 Screen will open. This is the Gateway for the NX 10 software. The NX 10 blank
screen looks like the figure shown below. There will be several tips displayed on the screen about
the special features of the current version. The Gateway also has the Standard Toolbar that will
allow you to create a new file or open an existing file. On the left side of the Gateway screen, there
is a toolbar called the Resource Bar that has menus related to different modules and the ability to
define and change the Role of the software, view History of the software use and so on. This will
be explained in detail later in this chapter.
2.1.2 Open a New File
Let’s begin by learning how to open a new part file in NX 10. To create a new file there are three
options.
 Click on the New button on top of the screen
OR
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 Go through the File drop-down menu at the top-left of the screen and click New
OR
 Press <Ctrl> + N
This will open a new session, asking for the type, name and location of the new file to be created.
There are numerous types of files in NX 10 to select from the Templates dialogue box located at
the center of the window. The properties of the selected file are displayed below the Preview on
the right side. Since we want to work in the modeling environment and create new parts, only
specify the units (inches or millimeters) of the working environment and the name and location of
the file. The default unit is millimeters.
 Enter an appropriate name and location for the file and click OK
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2.1.3 Open a Part File
There are several ways to open an existing file.
 Click on the Open or Open a Recent Part button on top of the screen
OR
 Go through the File drop-down menu at the top-left of the screen and click Open
OR
 Press <Ctrl> + O
The Open Part File dialog will appear. You can see the preview of the files on the right side of the
window. You can disable the Preview by un-clicking the box in front of the Preview button.
 Click Cancel to exit the window
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2.2 PRINTING, SAVING AND CLOSING FILES
2.2.1 Print an NX 10 Image
To print an image from the current display,
 Click File →Print
The following figure shows the Print dialog box. Here,
you can choose the printer to use or specify the number
of copies to be printed, size of the paper and so on.
You can also select the scale for all the three
dimensions. You can also choose the method of
printing, i.e. wireframe, solid model by clicking on the
Output drop down-menu as shown in the Figure on right
side
 Click Cancel to exit the window
2.2.2 Save Part Files
It is imperative that you save your work frequently. If
for some reasons, NX 10 shuts down and the part is not
saved, all the work will be lost. To save the part files,
 Click File →Save
There are five options to save a file:
Save: This option will save the part on screen with the
same name as given before while creating the part file.
Save Work Part Only: This option will only save the
active part on the screen.
Save As: This option allows you to save the part on screen using a different name and/or type. The
default type is .prt. However, you can save your file as IGES (.igs), STEP 203 (.stp), STEP 214
(.step), AutoCAD DXF (.dxf), AutoCAD DWG (.dwg), CATIA Model (.model) and CATIA V5
(.catpart).
Save All: This option will save all the opened part files with their existing names.
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Save Bookmark: This option will save a screenshot and context of the present model on the screen
as a .JPEG file and bookmarks.
2.2.3 Close Part Files
You can choose to close the parts that are
visible on screen by
 Click File →Close
If you close a file, the file will be cleared from
the working memory and any changes that are
not saved will be lost. Therefore, remember
to select Save and Close, Save As and Close,
Save All and Close or Save All and Exit. In
case of the first three options, the parts that
are selected or all parts will be closed but the
NX 10 session keeps on running.
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2.2.4 Exit an NX 10 Session
 Click File →Exit
If you have files open and have made changes to them without saving, the message will ask you if
you really want to exit.
 Select No, save the files and then Exit
2.3 NX 10 INTERFACE
The user interface of NX 10 is made very simple through the use of different icons. Most of the
commands can be executed by navigating the mouse around the screen and clicking on the icons.
The keyboard entries are mostly limited to entering values and naming files.
2.3.1 Mouse Functionality
2.3.1.1 Left Mouse Button (MB1)
The left mouse button, named Mouse Button 1 (MB1) in NX, is used for Selection of icons, menus,
and other entities on the graphic screen. Double clicking MB1 on any feature will automatically
open the Edit Dialog box. Clicking MB1 on an object enables the user to have quick access to
several options shown below. These options will be discussed in next chapters.
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2.3.1.2 Middle Mouse Button (MB2)
The middle mouse button (MB2) or the scroll button is used to Rotate the object by pressing,
holding and dragging. The model can also be rotated about a single axis. To rotate about the axis
horizontal to the screen, place the mouse pointer near the right edge of the graphic screen and
rotate. Similarly, for the vertical axis and the axis perpendicular to the screen, click at the bottom
edge and top edge of the screen respectively and rotate. If you keep pressing the MB2 at the same
position for a couple of seconds, it will fix the point of rotation (an orange circle symbol appears)
and you can drag around the object to view.
If it is a scroll button, the object can be zoomed in and out by scrolling. Clicking the MB2 will
also execute the OK command if any pop-up window or dialog box is open.
2.3.1.3 Right Mouse Button (MB3)
MB3 or Right Mouse Button is used to
access the user interface pop-up
menus. You can access the subsequent
options that pop up depending on the
selection mode and Application. The
figure shown below is in Sketch
Application. Clicking on MB3 when a
feature is selected will give the options
related to that feature (Object/Action
Menu).
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Clicking MB3 and holding the button will display a set of icons around the feature.
These icons feature the possible commands that can be applied to the feature.
2.3.1.4 Combination of Buttons
Zoom In /Out:
 Press and hold both MB1 and MB2 simultaneously and drag
OR
 Press and hold <Ctrl> button on the keyboard and then press and drag the MB2
OR
Pan:
 Press and hold both the MB2 and MB3 simultaneously and drag
OR
 Press and hold <Shift> button on the keyboard and press and drag the MB2
Shortcut to menus:
 Press and hold <Ctrl> + <Shift> and MB1, MB2 and MB3 to see shortcuts to Feature,
Direct Sketch, and Synchronous Modeling groups, respectively
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2.3.2 NX 10 Gateway
The following figure shows the typical layout of the NX 10 window when a file is opened. This is
the Gateway of NX 10 from where you can select any module to work on such as modeling,
manufacturing, etc. It has to be noted that these toolbars may not be exactly on the same position
of the screen as shown below. The toolbars can be placed at any location or position on the screen.
Look out for the same set of icons.
Quick Access Toolbar
Ribbon Bar
Top-border
Groups
Tabs
Command Finder
Resource Bar
Graphic Window
Cue Line
2.3.2.1 Ribbon Bar
The ribbon bar interface gives the user the ability to access the different commands easily without
reducing the graphics window area. Commands are organized in ribbon bars under different tabs
and groups for easy recognition and accessibility.
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For example in the ribbon bar shown in the figure above, we have home, curve, etc. tabs. In the
home tab, we have direct sketch, feature, synchronous modeling and surface groups. And in each
group, we have a set of featured commands.
2.3.2.2 Quick Access Toolbar
The quick access toolbar has most commonly used buttons (save, undo, redo, cut, copy, paste and
recent commands) to expedite the modeling process. You may easily customize these buttons as
shown in the figure below.
2.3.2.3 Command Finder
If you do not know where to find a command, use Command Finder. Let’s say we have forgotten
where the Styled Sweep is.
 Type sweep in the Command Finder
 Hover the mouse over Styled Sweep
 NX will show you the path to the command: Menu →Insert →Sweep →Styled Sweep
OR
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 Type sweep in the Command Finder
 Click on Styled Sweep in the Command Finder window
2.3.2.4 Top-border
The most important button in the top-border is the menu button. Most of the features and functions
of the software are available in the menu. The Selection Bar displays the selection options. These
options include the Filters, Components/Assembly, and Snap Points for selecting features. Most
common buttons in the View tab are also displayed in the Top-border.
2.3.2.5 Resource Bar
The Resource Bar features icons for a number of pages in one place using very little user interface
space. NX 10 places all navigator windows (Assembly, Constraint and Part) in the Resource Bar,
as well as the Reuse Library, HD3D Tools, Web Browser, History Palette, Process Studio,
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Manufacturing Wizards, Roles and System Scenes. Two of the most important widows are
explained below.
Part Navigator
 Click on the Part Navigator icon, the third
icon from the top on the Resource bar
The Part Navigator provides a visual representation
of the parent-child relationships of features in the
work part in a separate window in a tree type format.
It shows all the primitives, entities used during
modeling. It allows you to perform various editing
actions on those features. For example, you can use
the Part Navigator to Suppress or Unsuppress the
features or change their parameters or positioning
dimensions. Removing the green tick mark will
‘Suppress’ the feature. The software will give a
warning if the parent child relationship is broken by
suppressing any particular feature.
The Part Navigator is available for all NX
applications and not just for modeling. However, you can only perform feature-editing operations
when you are in the Modeling module. Editing a feature in the Part Navigator will automatically
update the model. Feature editing will be discussed later.
History
 Click on the History icon, the seventh from the top on the Resource bar
The History Palette provides fast access to recently opened files or other palette entries. It can be
used to reload parts that have been recently worked on or to repeatedly add a small set of palette
items to a model.
The History Palette remembers the last palette options that were used and the state of the session
when it was closed. NX stores the palettes that were loaded into a session and restores them in the
next session. The system does not clean up the History Palette when parts are moved.
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To re-use a part, drag and drop it from the History
Palette to the Graphics Window. To reload a part,
click on a saved session bookmark.
2.3.2.6 Cue Line
The Cue Line displays prompt messages that indicate
the next action that needs to be taken. To the right of
the Cue line, the Status Line is located which
displays messages about the current options or the
most recently completed function.
The Progress Meter is displayed in the Cue Line
when the system performs a time-consuming
operation such as loading a large assembly. The
meter shows the percentage of the operation that has
been completed. When the operation is finished, the
system displays the next appropriate cue.
2.3.3 Geometry Selection
You can filter the selection method, which facilitates
easy selection of the geometry in a close cluster. In
addition, you can perform any of the feature
operation options that NX 10 intelligently provides
depending on the selected entity. Selection of items can be based on the degree of the entity like,
selection of Geometric entities, Features and Components. The selection method can be opted by
choosing one of the icons in the Selection Toolbar.
2.3.3.1 Feature Selection
Clicking on any of the icons lets you select the features in the part file. It will not select the basic
entities like edges, faces etc. The features selected can also be applied to a part or an entire
assembly depending upon the requirement.
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Besides that, the filtering of the features can be further narrowed down by
selecting one of the desired options in the drop-down menu as shown in the
figure. For example, selecting Curve will highlight only the curves in the
screen. The default is No Selection Filter.
2.3.3.2 General Object Selection
Navigate the mouse cursor closer to the entity until it is highlighted with a
magenta color and click the left mouse button to select any geometric entity,
feature, or component.
If you want to select an entity that is hidden behind the displayed geometry,
place the mouse cursor roughly close to that area on the screen such that the
cursor ball occupies a portion of the hidden geometry projected on the
screen. After a couple of seconds, the ball cursor turns into a plus symbol
as shown in the figure. Click the left mouse button (MB1) to get a Selection
Confirmation dialog box as shown in the
following figure below. This QuickPick
menu consists of the list of entities
captured within the ball of the cursor. The
entities are arranged in ascending order of
the degree of the entity. For example,
edges and vertices are assigned lower
numbers while solid faces are given
higher numbers. By moving the cursor on
the numbers displayed, NX 10 will
highlight the corresponding entity on the screen in a magenta color.
2.3.4 User Preferences
 Choose Preferences on the Menu button (located to top left of the main window) to find
the various options available
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User Preferences are used to define the display parameters of
new objects, names, layouts, and views. You can set the layer,
color, font, and width of created objects. You can also design
layouts and views, control the display of object and view
names and borders, change the size of the selection ball,
specify the selection rectangle method, set chaining tolerance
and method, and design and activate a grid. Changes that you
make using the Preferences menu override any counterpart
customer defaults for the same functions.
2.3.4.1 User Interface
 Choose Preferences →User Interface to find the
options in the dialog box
The User Interface option customizes how NX works and
interacts to specifications you set. You can control the
location, size and visibility status of the main window,
graphics display, and information window. You can set the
number of decimal places (precision) that the system uses for
both input text fields and data displayed in the information
window. You can also specify a full or small dialog for file
selection. You can also set macro options and enable a
confirmation dialog for Undo operations.
•
The Layout tab allows you to select the User Interface Environment
•
The Touch tab lets you use touch screens
•
The Options tab allows you, among others, to set the precision level (in the Information
Window)
•
The Journal tab in the Tools allows you to use several programming languages
•
The Macro tab in the Tools allows you to set the pause while displaying animation
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2.3.4.2 Visualization
 Choose Preferences →Visualization to find the
options in the dialog box
This dialog box controls attributes that affect the display in
the graphics window. Some attributes are associated with
the part or with particular Views of the part. The settings for
these attributes are saved in the part file. For many of these
attributes, when a new part or a view is created, the setting
is initialized to the value specified in the Customer Defaults
file. Other attributes are associated with the session and
apply to all parts in the session. The settings of some of
these attributes are saved from session to session in the
registry. For some session attributes, the setting can be
initialized to the value specified by customer default, an
environment variable.
 Choose Preferences →Color Pallet to find the
options in the dialog box
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 Click on Preferences →Background to get
another pop up Dialog box. You can change
your background color whatever you want
The background color refers to the color of the
background of the graphics window. NX supports
graduated backgrounds for all display modes. You can
select background colors for Shaded or Wireframe
displays. The background can be Plain or Graduated.
Valid options for all background colors are 0 to 255.
You can change and observe the Color and
Translucency of objects.
 Click Preferences →Object
This will pop up a dialog window Object Preferences.
You can also apply this setting to individual entities of
the solid. For example, you can click on any particular
surface of the solid and apply the Display settings.
2.3.5 Applications
Applications can be opened using the File option
located at the top left corner of the main window OR
the Applications tab above the Ribbon bar. You can
select the type of application you want to run. For
example,
you can select Modeling, Drafting,
Assembly, and so on as shown in the figure. The default Application that starts when you open a
file or start a new file is Modeling. We will introduce some of these Application in the next
chapters.
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2.4 LAYERS
Layers are used to store objects in a file, and work like containers to collect the objects in a
structured and consistent manner. Unlike simple visual tools like Show and Hide, Layers provide
a permanent way to organize and manage the visibility and selectability of objects in your file.
2.4.1 Layer Control
With NX 10, you can control whether objects are visible or selectable by using Layers. A Layer is
a system-defined attribute such as color, font, and width that all objects in NX 10 must have. There
are 256 usable layers in NX 10, one of which is always the Work Layer. Any of the 256 layers can
be assigned to one of four classifications of status.
•
Work
•
Selectable
•
Visible Only
•
Invisible
The Work Layer is the layer that objects are created ON and is
always visible and selectable while it remains the Work Layer.
Layer 1 is the default Work Layer when starting a new part file.
When the Work Layer is changed to another type of layer, the
previous Work Layer automatically becomes Selectable and can
then be assigned a status of Visible Only or Invisible.
The number of objects that can be on one layer is not limited. You
have the freedom to choose whichever layer you want to create
the object on and the status of that layer.
To assign a status to a layer or layers,
 Choose View →Layer Settings
However, it should be noted that the use of company standards in
regards to layers would be advantageous to maintain a consistency
between files.
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2.4.2 Commands in Layers
We will follow simple steps to practice the commands in Layers. First, we will create two objects
(Solids) by the method as follows. The details of Solid Modeling will be discussed in the next
chapter. The solids that we draw here are only for practice in this chapter.
 Choose File →New
Name the file and choose a folder in which to save it. Make
sure you select the units to be millimeters in the drop-down
menu. Choose the file type as Model
 Choose
Menu
→Insert
→Design
Feature
→Cone
 Choose Diameter and Height under Type
 Click OK
 Right-click on the screen and choose Orient View
→Trimetric
 Right-click on the screen and choose Rendering
Style →Shaded
You will be able to see a solid cone similar to the picture
on right.
Now let us practice some Layer Commands.
 Choose View →Move to Layer
You will be asked to select an object
 Move the cursor on to the Cone and click on it so that it becomes highlighted
 Click OK
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 In the Destination Layer or Category space at the top of the window, type 25 and Click
OK
The Cone has now gone to the 25th layer. It can no longer be
seen in Layer 1.
 To see the Cone, click View →Layer Settings
 You can see that Layer 25 has the object whereas the
default Work Layer 1 has no objects.
The Cone will again be seen on the screen. Save the file as we
will be using it later in the tutorial.
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2.5 COORDINATE SYSTEMS
There are different coordinate systems in NX. A three-axis symbol is used to identify the
coordinate system.
2.5.1 Absolute Coordinate System
The Absolute Coordinate System is the coordinate system from which
all objects are referenced. This is a fixed coordinate system and the
locations and orientations of every object in NX 10 modeling space are
related back to this system. The Absolute Coordinate System (or
Absolute CSYS) also provides a common frame of reference between
part files. An absolute position at X=1, Y=1, and Z=1 in one part file is
the same location in any other part file.
The View Triad on the bottom-left of the Graphics window is ONLY a visual
indicator that represents the ORIENTATION of the Absolute Coordinate System
of the model.
2.5.2 Work Coordinate System
The Work Coordinate System (WCS) is what you will use for construction when you want to
determine orientations and angles of features. The axes of the WCS are denoted XC, YC, and ZC.
(The “C” stands for “current”). It is
possible to have multiple coordinate
systems in a part file, but only one of them
can be the work coordinate system.
2.5.3 Moving the WCS
Here, you will learn how to translate and
rotate the WCS.
 Choose Menu →Format →WCS
2.5.3.1 Translate the WCS
This procedure will move the WCS origin
to any point you specify, but the
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orientation (direction of the axes) of the WCS will remain the same.
 Choose Menu →Format →WCS →Origin
The Point Constructor dialog is displayed. You either can
specify a point from the drop down menu at the top of the
dialog box or enter the X-Y-Z coordinates in the XC, YC,
and ZC fields.
The majority of the work will be in relation to the Work
Coordinate System rather than the Absolute Coordinate
System. The default is the WCS.
2.5.3.2 Rotate the WCS
You can also rotate the WCS around one of its axes.
 Choose Menu → Format →WCS →Rotate
The dialog shows six different ways to rotate the WCS
around an axis. These rotation procedures follow the righthand rule of rotation. You can also specify the angle to which the
WCS be rotated.
You can save the current location and orientation of the WCS to use
as a permanent coordinate system.
 Choose Menu →Format →WCS →Save
2.6 TOOLBARS
Toolbars contain icons, which serve as shortcuts for many functions.
The figure on the right shows the main Toolbar items normally
displayed. However, you can find many more icons for different
feature commands, based on the module selected and how the
module is customized.
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 Right-Clicking anywhere on the existing toolbars gives a list of other Toolbars. You can
add any of the toolbars by checking them.
Normally, the default setting should be sufficient for most operations but during certain operations,
you might need additional toolbars. If you want to add buttons pertaining to the commands and
toolbars,
 Click on the pull-down arrow on any of the Toolbars and choose Customize.
This will pop up a Customize dialog window with all the Toolbars and commands pertaining to
each Toolbar under Commands tab. To add a command,
 Choose a category and drag the command from the Commands list to the desired location.
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You can customize the settings of your NX 10 interface by
clicking on the Roles tab on the Resource Bar.
The Roles tab has different settings of the toolbar menus
that are displayed on the NX 10 interface. It allows you to
customize the toolbars you desire to be displayed in the
Interface.
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CHAPTER 3 – TWO DIMENSIONAL SKETCHING
In this chapter, you will learn how to create and edit sketches in NX 10. You can directly create a
sketch on a Plane in Modeling application. In most cases, Modeling starts from a 2D sketch and
then Extrude, Revolve or Sweep the sketch to create solids. Many complex shapes that are
otherwise very difficult to model can easily be drawn by sketching. In this chapter, we will see
some concepts of sketching and then proceed to sketch and model some parts.
3.1 OVERVIEW
An NX 10 sketch is a named set of curves joined in a string that when swept, form a solid. The
sketch represents the outer boundary of that part. The curves are created on a plane in the sketcher.
In the beginning, these curves are drawn without any exact dimensions. Then, Dimensional
Constraints as well as Geometric Constraints are applied to fully constrain the sketch. These will
be discussed in detail later in this chapter.
After sketching is completed, there are different ways to use them to generate 3D parts:
•
A sketch can be revolved
•
A sketch can be extruded
•
A sketch can be swept along a guide (line):
Features created from a sketch are associated with it; i.e., if
the sketch changes so do the features.
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The advantages of using sketching to create parts are:
•
The curves used to create the profile outline are very flexible and can be used to model
unusual shapes.
•
The curves are parametric, hence associative and they can easily be changed or removed.
•
If the plane in which the sketch is drawn is changed, the sketch will be changed
accordingly.
•
Sketches are useful when you want to control an outline of a feature, especially if it may
need to be changed in the future. Sketches can be edited very quickly and easily.
3.2 SKETCHING ENVIRONMENT
In NX 10 you can create sketch using two ways. The
first method creates the Sketch in the current
environment and application. For this,
 Choose Menu →Insert →Sketch
In the other method you can create Sketch using
 Choose Sketch in Home toolbar
In either case, a dialog box pop-ups asking you to
define the Sketch Plane. The screen will display the
sketch options. You can choose the Sketch Plane,
direction of sketching and type of plane for sketching.
When you create a sketch using the Create Sketch dialog box, you can choose the plane on which
the sketch can be created by clicking on the coordinate frame as shown. This will highlight the
plane you have selected. The default plane selected is XC-YC. However,
you can choose to sketch on another plane. If there are any solid features
created in the model beforehand, any of the flat surfaces can also be used
as a sketching plane.
 Choose the XC-YC plane and click OK
The sketch plane will appear and the X-Y directions will be marked.
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The main screen will change to the Sketching Environment. The XY plane is highlighted as the
default plane for sketching. This is the basic sketch window. There is also a special Sketch Task
Environment in NX 10 which displays all sketch tools in the main window. For accessing the
Sketch Task Environment,
 Click the More option in the direct sketch tool bar area
 Click on Open in Sketch Task Environment as shown below
There are three useful options next to the Finish Flag. You can change
the name of the sketch in the box. The next one is Orient to Sketch
which orients the view to the plane of the sketch. If the model file is
rotated during the process of sketching, click on this icon to view the
sketch on a plane parallel to the screen Reattach attaches the sketch to a different planar face,
datum plane, or path, or changes the sketch orientation. It allows you to reattach the sketch to the
desired plane without recreating all the curves, dimensions, and constraints.
3.3 SKETCH CURVE TOOLBAR
This toolbar contains icons for creating the common types of
curves and spline curves, editing, extending, trimming,
filleting etc. Each type of curve has different methods of
selection and methods of creation. Let us discuss the most
frequently used options.
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Profile
This option creates both straight lines as well as arcs depending on the icon you select in the popup toolbar. You can pick the points by using the coordinate system or by entering the length and
angle of the line as shown in the following figures.
Line
This option will selectively create only straight lines.
Arc
This option creates arcs by either of two methods. The first option creates arc with three sequential
points as shown below.
The second option creates the arc with a center point, radius and sweep angle or by center point
with a start point and end point. The illustration is shown below.
Circle
Creating a circle is similar to creating an arc, except that circle is closed.
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Quick Trim
This trims the extending curves from the points of intersection of the curves. This option reads
every entity by splitting them if they are intersected by another entity and erases the portion
selected.
Studio Spline
You can create basic spline curves (B-spline and Bezier) with poles or through points with the
desired degree of the curve. The spline will be discussed in detail in the seventh chapter (Freeform
Features).
3.4 CONSTRAINTS TOOLBAR
All the curves are created by picking points. For example, a straight line is created with two points.
In a 2D environment, any point has two degrees of freedom, one along X and another along Y
axis. The number of points depends on the type of curve being created. Therefore, a curve entity
has twice the number of degrees of freedom than the number of points it comprises. These degrees
of freedom can be removed by creating a constraint with a fixed entity. In fact, it is recommended
that you remove all these degrees of freedom (making the sketch Fully Constrained) by relating
the entities directly or indirectly to the fixed entities. It can be done by giving dimensional or
geometric properties like Parallelity, Perpendicularity, etc.
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In NX 10 smart constraints are applied automatically, i.e. automatic dimensions or geometrical
constraints are interpreted by NX 10. You can turn this option off by clicking on Continuous Auto
Dimensioning as shown below. The following paragraphs show how to manually apply constraints.
Dimensional Constraints
The degrees of freedom can be eliminated by giving dimensions with fixed entities like axes,
planes, the coordinate system or any existing solid geometries created in the model. These
dimensions can be linear, radial, angular etc. You can edit the dimensional values at any time
during sketching by double-clicking on the dimension.
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Geometric Constraints
Besides the dimensional constraints, some geometric constraints can be given to eliminate the
degrees of freedom. They include parallel, perpendicular, collinear, concentric, horizontal,
vertical, equal length, etc. The software has the capability to find the set of possible constraints for
the selected entities. As an example, a constraint is applied on the line in the below picture to be
parallel to the left side of the rectangle (the line was originally at an angle with the rectangle).
Display Sketch Constraints
Clicking this icon will show all the options pertaining to the entities in that particular sketch in
white.
Show/Remove Constraints
This window lists all the constraints and types of constraints pertaining to any entity selected. You
can delete any of the listed constraints or change the sequence of the constraints.
The number of degrees of freedom that are not constrained are displayed in the Status Line. All
these should be removed by applying the constraints to follow a disciplined modeling.
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3.5 EXAMPLES
3.5.1 Arbor Press Base
 Create a new file and save it as Arborpress_base.prt
 Click on the Sketch button and click OK
 Choose Menu →Insert →Sketch Curve →
Profile or click on the Profile icon in the Direct
Sketch
group
(remember
to
deactivate
Continuous Dimensioning)
 Draw a figure similar to the one shown on right.
While making continuous sketch, click on the Line
icon on the Profile dialog box to create straight
lines and the Arc icon to make the semicircle.
(Look at the size of the XY plane in the figure. Use
that perspective for the approximate zooming).
Once the sketch is complete, we constrain the sketch. It is
better to apply the geometric constraints before giving the
dimensional constraints.
 Choose Insert →Geometric Constraints or click
on the Constraints icon in the side toolbar
Now we start by constraining between an entity in the sketch and a datum or a fixed reference.
First, place the center of the arc at the origin. This creates a reference for the entire figure. We can
use the two default X and Y axes as a datum reference.
 Select Point on Curve
constraint
 Select the Y-axis and then the center of the arc
 Repeat the same procedure to place the center of the arc on the X-axis
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Do not worry in case the figure gets crooked. The figure will come back to proper shape once all
the constraints are applied. However, it is better to take into consideration the final shape of the
object when you initially draw the unconstrained figure.
 Select the two slanted lines and make them Equal Length
 Similarly select the two long vertical lines and make them Equal Length
 Select the bottom two horizontal lines and make them Collinear and then click on the same
lines and make them Equal Length
If you DO NOT find the two Blue circles (Tangent Constraints) near the
semicircle as shown in the figure, follow the below steps. Otherwise, you
can ignore this.
 Select the circular arc and one of the two vertical lines connected to its endpoints
 Select the Tangent icon
If the arc and line is already tangent to each other, the icon will be grayed out. If that is the case
 Click on Edit →Selection →Deselect All. Repeat the same procedure for the arc and the
other vertical line.
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 Select the two vertical lines and make them Equal
 Similarly select the two small horizontal lines at the top of the profile and make them
Collinear and Equal
 Similarly select the two vertical lines and make them Equal
Note: At times after applying a constraint, the geometric
continuity of the sketch may be lost like shown. In such
conditions, click the exact end points of the two line and
click the Coincident constraint as shown.
So far, we have created all the Geometric constraints. Now we have to create the Dimensional
constraints. If there is any conflict between the Dimensional and Geometric constraints, those
entities will be highlighted in yellow.
 Choose the Rapid Dimension icon
in the Constraints toolbar
 Add on all the dimensions as shown in the following figure without specifying the values
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For example, to create a dimension for the top two corners,
 Click somewhere near the top of the two diagonal lines to select them
While dimensioning, if you find the dimensions illegible, but do not worry about editing the
dimensions now.
Now we edit all the dimension values one by one. It is highly recommended to start editing from
the biggest dimension first and move to the smaller dimensions. Once enough number of
dimensions are provided, sketch color changes indicating it is fully defined.
 Edit the values as shown in the figure below. Double click on each dimension to change
the values to the values as shown in figure below
 Click on the Finish Flag
on the top left corner or bottom right of the screen when
you are finished
 Click on the sketch and select Extrude (this Feature is explained in details in the next
sections)
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 Extrude this sketch in the Z-direction by 60 mm
 Save and close the file
3.5.2 Impeller Lower Casing
 Create a new file in inches and save it as Impeller_lower_casing.prt
 Click Menu →Insert →Sketch In Task Environment or click Sketch In Task
Environment icon
from the ribbon bar
 Set the sketching plane as the XC-YC plane
 Make sure the Profile window is showing and draw the following curve
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Line 2
Curve 1
Line 1
Curve 2
 Create a point at the origin (0, 0, 0) by clicking the plus sign in the Direct Sketch group
Next, we will constrain the curve
 Click on the Geometric Constraints icon
 Select the point at the origin and click on the Fixed
constraint icon
(if you cannot see this icon, click
on Settings and check it as shown on the right)
 Make all of the curve-lines and curve-curve joints
Tangent
 Apply the dimensional constraints as shown in the
figure below
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 Select all the dimensions.
 Right click and Hide the dimensions
 Choose Menu →Edit →Move Object or choose
Move Curve from the ribbon bar
 Select all the curves. You should see 4 objects being
selected in Select Object
 Specify the Motion to be Distance
 Choose YC-Direction in the Specify Vector
 Enter the Distance to be 0.5 inch
 In the Result dialog box make sure you the click on
the Copy Original radio button
 Click OK
 Then join the end-points at the two ends using the
basic curves to complete the sketch
The sketch is ready.
 Choose Edit →Move Object or choose Move Curve from the ribbon bar
 Select the outer curve. Be sure to select all the four parts of the curve
 Move the lower curve in the Y-direction by -1.5 inches. This is the same as translating it
in the negative YC-direction by 1.5 inches
This will form a curve outside the casing.
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 Using straight lines join this curve with the inside curve of the casing
It will form a closed chain curve as shown.
Now we will create the curve required for outside of the casing on the smaller side which will form
the flange portion.
 Choose Edit → Move Object
 Select the outer line as shown in the figure below
 Move the lower curve in the XC-direction by -0.5 inches. This is the same as translating it
in the negative XC-direction by 0.5 inches
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 Using straight lines join the two lines as shown in the figure on right side
 Click on the Finish Flag
 Save and Close the file
We will use this sketching in the next chapter to model the Impeller Lower
Casing.
3.5.3 Impeller
 Create a new file in inches and save it as Impeller_impeller.prt
 Click on Sketch
 Set the sketching plane as the XC-YC plane and click OK
 Click on Menu →Insert →Datum/Point →Point or
click Point from Direct Sketch group in the ribbon bar
 Create two Points, one at the origin (0, 0, 0) and one at
(11.75, 6, 0)
 Click on the Arc icon on the side toolbar and click on the Arc by Center and Endpoints
icon
in the pop-up toolbar
 Click on the point at the origin and create an arc with a radius of 1.5 similar to the one
shown in the figure below
 Click on the point at (11.75, 6, 0) and create an arc with
a radius of 0.5
 Click on the Arc by 3 Points icon
in the pop-up
toolbar
 Select the top endpoints of the two arcs you just created
and click somewhere in between to create another arc that connects them. Do the same for
the bottom endpoints
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 Click on the Constraints icon in the side toolbar and
make sure that all the arcs are Tangent to one another
at their endpoints
 Click on the point at the origin and click on the Fixed
icon
 Then click on the Rapid Dimension icon
 Give the Radius dimensions for each arc. Edit dimensions so that the two arcs on the end
are 1.5 and 0.5 inches and the two middle arcs are 18 and 15 inches as shown in the figure
below
 Click on the Finish Flag
 Save and Close the file.
We will use this sketching in the next chapter to
model the Impeller.
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CHAPTER 4 – THREE DIMENSIONAL MODELING
This chapter discusses the basics of three dimensional modeling in NX 10. We will discuss what
a feature is, what the different types of features are, what primitives are and how to model features
in NX 10 using primitives. This will give a head start to the modeling portion of NX 10 and develop
an understanding of the use of Form Features for modeling. Once these feature are introduced, we
will focus on Feature Operations which are functions that can be applied to the faces and edges
of a solid body or features you have created. These include taper, edge blend, face blend, chamfer,
trim, etc. After explaining the feature operations, the chapter will walk you through some
examples.
In NX 10, Features are a class of objects that have a defined parent. Features are associatively
defined by one or more parents and the order of their creation and modification retain within the
model, thus capturing it through the History. Parents can be geometrical objects or numerical
variables. Features include primitives, surfaces and/or solids and certain wire frame objects (such
as curves and associative trim and bridge curves). For example, some common features include
blocks, cylinders, cones, spheres, extruded bodies, and revolved bodies.
Commonly Features can be classified as following
-
Body: A class of objects containing solids and sheets
-
Solid Body: A collection of faces and edges that enclose a volume
-
Sheet Body: A collection of one or more faces that do not enclose a volume
-
Face: A region on the outside of a body enclosed by edges
4.1 TYPES OF FEATURES
There are six types of Form Features: Primitives, Reference features, Swept features, Remove
features, Extract features, and User-defined features. Similar to previous versions, NX 10 stores
all the Form Features under the Insert menu option. The form features are also available in the
Form Features Toolbar.
 Click Insert on the Menu
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As you can see, the marked menus in the figure on the right side contain the commands of Form
Features. The Form Feature icons are grouped in the Home Toolbar as shown below. You can
choose the icons that you use frequently.
 Click on the drop down arrow in Home Toolbar
 Choose Feature Group
4.1.1 Primitives
They let you create solid bodies in the form of generic building shapes. Primitives include:
•
Block
•
Cylinder
•
Cone
•
Sphere
Primitives are the primary entities. Hence, we will begin with a short description of primitives and
then proceed to modeling various objects.
4.1.2 Reference Features
These features let you create reference planes or reference axes. These references can assist you
in creating features on cylinders, cones, spheres and revolved solid bodies.
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 Click on Menu →Insert →Datum/Point or click on Datum Plane in Feature group in
the ribbon bar to view the different Reference Feature options: Datum Plane, Datum
Axis, Datum CSYS, and Point
4.1.3 Swept Features
These features let you create bodies by extruding or revolving sketch geometry. Swept Features
include:
•
Extruded Body
•
Revolved Body
•
Sweep along Guide
•
Tube
•
Styled Sweep
To select a swept feature you can do the following:
 Click on Insert →Design Feature for Extrude and Revolve or click on Extrude in
Feature group in the ribbon bar
OR
 Click on Insert →Sweep or click on More in Feature group in the ribbon bar to find all
the options available including Sweep
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4.1.4 Remove Features
Remove Features let you create bodies by removing
solid part from other parts.
 Click on Insert →Design Feature
Remove Features include:
•
Hole
•
Pocket
•
Slot
•
Groove
4.1.5 Extract Features
These features let you create bodies by extracting
curves, faces and regions. These features are widely
spaced under Associative Copy and Offset/Scale
menus. Extract Features include:
•
Extract
•
Solid to Shell
•
Thicken Sheet
•
Bounded plane
•
Sheet from curves
 Click on Insert →Associative Copy →Extract for Extract options or click on More in
Feature group in the ribbon bar to find Extract Geometry
 Click on Insert →Offset/Scale for Solid to Shell and Thicken Sheet Assistant or click on
More in Feature group in the ribbon bar to find Offset/Scale options
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 Click on Insert →Surface for Bounded Plane and Sheet from curves
4.1.6 User-Defined features
These features allow you to create your own form features to automate commonly used design
elements. You can use user-defined features to extend the range and power of the built-in form
features.
 Click on Insert →Design Feature →User Defined
4.2 PRIMITIVES
Primitive features are base features from which many other features can be created. The basic
primitives are blocks, cylinders, cones and spheres. Primitives are non-associative which means
they are not associated to the geometry used to create them.
Note that usually Swept Features are used to create
Primitives instead of the commands mentioned here.
4.2.1 Model a Block
 Create
a
new
file
and
name
it
as
Arborpress_plate.prt
 Choose Insert →Design Feature →Block or click
on the Block icon in the Form Feature Toolbar
The Block window appears. There are three main things to
define a block. They include the Type, Origin and the
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Dimensions of the block. To access the Types, scroll the drop-down menu under Type. There are
three ways to create a block primitive:
•
Origin and Edge Lengths
•
Height and Two Points
•
Two Diagonal Points
 Make sure the Origin and Edge Lengths method is selected
Now, we will choose the origin using the Point Constructor:
 Click on the Point Dialog icon under the Origin
The Point Constructor box will open. The XC, YC, ZC
points should have a default value of 0.
 Click OK
The Block window will reappear again.
 Type the following dimensions in the window
Length (XC) = 65 inches
Width (YC) = 85 inches
Height (ZC) = 20 inches
 Click OK
If you do not see anything on the screen,
 Right-click and select FIT. You can also press <Ctrl> + F
 Right-click on the screen and click on Orient View →Trimetric
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You should be able to see the complete plate solid model. Save and close the part file.
4.2.2 Model a Shaft
We will now model a shaft having two cylinders and one cone joined together.
 Create a new file and save it as Impeller_shaft.prt
 Choose Insert →Design Feature →Cylinder or
click on More in Feature group in the ribbon bar
to find Cylinder in Design Feature section
Similar to the Block, there are three things that need to be
defined to create a cylinder: Type, Axis & Origin, and
Dimensions.
A Cylinder can be defined by two types which can be
obtained by scrolling the drop-down menu under Type
•
Axis, Diameter, and Height
•
Arc and Height
 Select Axis, Diameter, and Height
 Click on the Vector Constructor icon next to
Specify Vector and select the ZC Axis icon
 Click on the Point Dialog icon next to Specify
Point to set the origin of the cylinder
 Set all the XC, YC, and ZC coordinates to be 0
You can see that the selected point is the origin of WCS
 In the next dialog box of the window, type in the following values
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Diameter = 4 inches
Height = 18 inches
 Click OK
 Right-click on the screen, choose Orient View →Isometric
The cylinder will look as shown on the right. Now we will create a cone at
one end of the cylinder.
 Choose Insert →Design Feature →Cone or click on More in
Feature group in the ribbon bar to find Cone in Design Feature
section
Similar to Block and Cylinder, there are various ways to create a cone which
can be seen by scrolling the drop-down menu in the Type box.
•
Diameters and Height
•
Diameters and Half Angle
•
Base Diameter, Height, and Half Angle
•
Top Diameter, Height, and Half Angle
•
Two Coaxial Arcs
 Select Diameters and Height
 Click on the Vector Constructor icon next to
Specify Vector
 Choose the ZC-Axis icon so the vector is
pointing in the positive Z direction
 Click on the Point Constructor icon next to
Specify Point to set the origin of the cylinder.
The Point Constructor window will appear next.
 Choose the Arc/Ellipse/Sphere Center icon on
the dialog box and click on the top circular edge
of the cylinder
OR
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 For the Output Coordinates, type in the following values:
XC = 0
YC = 0
ZC = 18
 Click OK
 In the Cone Window, type in the following values:
Base Diameter = 4 inches
Top Diameter = 6 inches
Height = 10 inches
 On the Boolean Operation window, choose Unite and
select the cylinder
 Click OK
Now the cone will appear on top of the cylinder. The shaft is as
shown on right.
Now we will create one more cylinder on top of the cone.
 Repeat the same procedure as before to create another Cylinder. The vector should be
pointing in the positive ZC-direction. On the Point Constructor window, again click on
the Center icon and construct it at the center point of the base of the cone. The cylinder
should have a diameter of 6 inches and a height of 20 inches. Unite the cylinder with the
old structure.
The complete shaft will look as shown on the right. Remember to save the model.
4.3 REFERENCE FEATURES
4.3.1 Datum Plane
Datum Planes are reference features that can be
used as a base feature in building a model. They
assist in creating features on cylinders, cones,
spheres, and revolved solid bodies which do not
have a planar surface and also aid in creating
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features at angles other than normal to the faces of the target solid. We will follow some simple
steps to practice Reference Features. For starters, we will create a Datum Plane that is offset from
a face as shown in the figure below.
 Open the model Arborpress_plate.prt
 Choose Insert →Datum/Point →Datum Plane
The Datum Plane dialog can also be opened by clicking the icon as shown in the figure below
from the Feature Toolbar.
The Datum Plane window allows you to choose the method of selection. However, NX 10 is smart
enough to judge the method depending on the entity you select if you keep in Inferred option,
which is also the Default option.
 Click on the top surface of the block so that it becomes highlighted
The vector displays the positive offset direction that the datum plane will be created in. If you had
selected the bottom face, the vector would have pointed downward, away from the solid.
 Insert the Offset Distance value as 15 inches in the dialog box and click OK
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 If you don’t see the complete model and plane, right-click and select FIT
4.3.2 Datum Axis
In this part, you are going to create a Datum Axis. A Datum Axis is a reference feature that can be
used to create Datum Planes, Revolved Features, Extruded Bodies, etc. It can be created either
relative to another object or as a fixed axis (i.e., not referencing, and not constrained by other
geometric objects).
 Choose Insert →Datum/Point →Datum Axis
The Datum Axis dialog can also be opened by clicking the icon as shown in
the figure below from the Feature toolbar.
The next window allows you to choose the method of selecting the axis.
However, NX 10 can judge which method to use depending on the entity you
select.
There are various ways to make a Datum Axis. They include Point and
Direction, Two Points, Two Planes, etc.
 Select the two points on the block as shown in the figure
on the right
 Click OK
The Datum Axis will be a diagonal as shown.
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4.4 SWEPT FEATURES
Two important Swept Features (Extrude and Revolve) are introduced here using a practical
example which is the continuation of the lower casing of the impeller which we started in the
previous chapter.
 Open the Impeller_lower_casing.prt
In the previous section, we finished the two dimensional sketching of this part and it should look
similar to the below figure.
 Click on Insert →Design Feature →Revolve
OR
 Click on the Revolve button in the Feature Group
Make sure that the Selection Filter is set to Single Curve as shown below on the Selection Filter
Toolbar
 Click on each of the 10 curves as shown in the next figure
 In the Axis dialog box , in the Specify Vector option choose the Positive XC-direction
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 In the Specify Point option, enter the coordinates (0, 0, 0) so the curve revolves around
XC-axis with respect to the origin
 Keep the Start Angle as 0 and enter 180 as the
value for the End Angle
 Click OK
The solid is shown on the right. Now, we will create
edges.
 Click on Insert →Design Feature →Extrude
OR
 Click on the Extrude button in the Feature
Group
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 Select the outer curve of the casing as shown in the figure below (again make sure that the
Selection Filter is set to Single Curve).
Note: In case you are not able to select the proper lines, left-click and
hold the mouse button and you will see a dialog box pop-up as shown
which will provide you the options of which curve to select.
 Extrude this piece in the negative Z-direction by 0.5 inches
The final solid will be seen as follows.
We will now use the Mirror option to create an edge on the other side.
 Choose Edit →Transform
 Select the solid edge as shown. For this
you will have to change the Filter in the
dialog box to Solid Body
 Click OK
 Choose Mirror Through a Plane
 Select the Center Line as shown below
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 Click OK
 Select Copy
 Click Cancel
The edge will be mirrored to the other side as shown below.
We will now create a flange at the smaller opening of the casing as shown.
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 Click on Insert →Design Feature →Revolve
Again make sure that the Selection Filter is set to Single Curve. The default Inferred Curve option
will select the entire sketch instead of individual curves.
 Revolve this rectangle in the positive XC-direction relative to the Origin just like for the
casing. The End Angle should be 180
This will form the edge as shown below.
The lower casing is complete. Save the model.
4.5 REMOVE FEATURES
Remove Features allow you to remove a portion of the existing object to create an object with
additional features that are part of the design. These are illustrated below.
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4.5.1 General Hole
This option lets you create Simple, Counterbored, Countersunk and Tapered holes in solid bodies.
 Open the file Arborpress_plate.prt
 Choose Insert →Design Features →Hole
OR
 Click on the icon in the Feature Toolbar as shown
The Hole window will open. There are various selections that need to be
done prior to making the holes. First you need to select the Type of the hole.
 Select the default General Hole
Next, you need to define the points at which you need to make the
holes.
 Click on the Sketch icon in the Position dialog box and
choose the top face of the plate as the Sketch Plane
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 Click OK
This will take you the Sketch Plane.
 Click on the Point Dialog icon and specify all the points as given in the table below
X
Y
Z
11.25
10.00
0.00
32.50
23.50
0.00
53.75
10.00
0.00
11.25
75.00
0.00
32.50
61.50
0.00
53.75
75.00
0.00
 Click OK after you enter the coordinates of each point
 Click Close once you have entered all the points
 Click on Finish flag in the top left corner of the window
This will take you out of the Sketch mode and bring back to the
original Hole window on the graphics screen.
 In the Form dialog, choose the default option of
Simple Hole
 Enter the following values in the Dimensions
window
Diameter = 8 inches
Depth = 25 inches
Tip Angle = 118 degrees
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 Choose Subtract in the Boolean dialog box and click OK
Make sure to save the model.
4.5.2 Pocket
This creates a cavity in an existing body.
 Create a Block using default values
 Choose Insert →Design Features →Pocket
 Select Rectangular
 Select the Face that you want to create the Pocket on
it
 Select a Vertical Face to use as the reference for
dimensioning
 Enter the dimensions of the Pocket as shown
 Change the Positioning if you want
4.5.3 Slot
This option lets you create a passage through or into a solid
body in the shape of a straight slot. An automatic subtract is
performed on the current target solid. It can be rectangular, Tslot, U-Slot, Ball end or Dovetail. An example is shown on
the right.
4.5.4 Groove
This option lets you create a groove in a solid body, as if a
form tool moved inward (from an external placement face) or outward (from an
internal placement face) on a rotating part, as with a turning operation. An
example is shown on the right.
Note: Pocket, Slot, and Groove features are not commonly used in practice. All
the models created using these features can be modeled using 2D Sketches and
Extrude/Revolve.
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4.6 FEATURE OPERATIONS
Feature Operations are performed on the basic Form Features to smooth corners, create tapers,
make threads, do instancing and unite or subtract certain solids from other solids. Some of the
Feature Operations are explained below.
4.6.1 Edge Blend
An Edge Blend is a radius blend that is tangent to the blended faces. This
feature modifies a solid body by rounding selected edges. This command
can be found under Insert →Detail Feature →Edge Blend. You can also
click on its icon in the Feature Group. You need to select the edges to be
blended and define the Radius of the Blend as shown below.
Similar to Edge Blend you can also do a Face Blend by selecting two faces.
4.6.2 Chamfer
The Chamfer Function operates very similarly to the Blend Function by adding or subtracting
material relative to whether the edge is an outside chamfer or an inside chamfer. This command
can be found under Insert →Detail Feature →Chamfer. You can also click on its icon in the
Feature Group. You need to select the edges to be chamfered and define the Distance of the
Chamfer as shown below.
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4.6.3 Thread
Threads can only be created on cylindrical faces. The Thread Function lets you create Symbolic
or Detailed threads (on solid bodies) that are right or left handed, external or internal, on cylindrical
faces such as Holes, Bosses, or Cylinders. It also lets you select the method of creating the threads
such as cut, rolled, milled or ground. You can create different types of threads such as metric,
unified, acme and so on. To use this command, go to Insert →Design Feature →Thread. An
example of a Detailed Thread is shown below.
For Threaded Holes, it is recommended to use the
Threaded Hole command instead of the Thread
command: Insert →Design Feature →Hole
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4.6.4 Trim Body
A solid body can be trimmed by a
Sheet Body or a Datum Plane. You
can use the Trim Body function to
trim a solid body with a sheet body
and at the same time retain
parameters and associativity. To
use this command, go to Insert
→Trim →Trim Body or click on its
icon in the Feature Group. An
example is shown on the right.
4.6.5 Split Body
A solid body can be split into two
similar to trimming it. It can be
done by a plane or a sheet body. To
use this command, go to Insert
→Trim →Split Body or click on its
icon in the Feature Group. An
example is shown on the right.
4.6.6 Mirror
Mirror is a type of Associative Copy in which a solid body is created by mirroring the body with
respect to a plane. To use this command, go to Insert →Associative Copy →Mirror Feature or
click on its icon in the Feature Group. An example is shown below.
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4.6.7 Pattern
A Design Feature or a Detail Feature can be made into dependent copies in the form of an Array.
It can be Linear, Circular, Polygon, Spiral, etc. This particularly helpful feature saves plenty of
time and modeling when you have similar features. For example threads of a gear or holes on a
mounting plate, etc. This command can be found under Insert →Associative Copy →Pattern
Feature. You can also click on its icon in the Feature Group. An example is shown below.
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4.6.8 Boolean Operations
There are three types of Boolean Operations: Unite, Subtract,
and Intersect. These options can be used when two or more solid
bodies share the same model space in the part file. To use this
command, go to Insert → Combine or click on their icons in the
Feature Group. Consider two solids given: a block and a
cylinder are next to each other as shown below.
4.6.8.1 Unite
The unite command adds the Tool body with the Target body. For the above example, the output
will be as follows if Unite option is used.
4.6.8.2 Subtract
When using the subtract option, the Tool Body is subtracted from the
Target Body. The following would be the output if the Block is used
as the Target and the Cylinder as the Tool.
4.6.8.3 Intersect
This command leaves the volume that is common to both the Target
Body and the Tool Body. The output is shown below.
4.6.9 Move
If you want to Move an object with respect to a fixed entity,
 Click on Edit →Move Object
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You can select the type of motion from the Motion drop-down menu. The default option is
Dynamic. With this you can move the object in any direction. There are several other ways of
moving the object.
If you choose Distance you can move the selected object in the X-Y-Z direction by the distance
that you enter.
 Click on Specify Vector and select the direction.
 Type 5 in the Distance box. This will translate the cylinder a distance of 5 inches along
X-Axis
 Click OK
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As you can see, we have moved the cylinder in the X-direction. Similarly, we can also copy the
cylinder by a specified distance or to a specified location by selecting the Copy Original option in
the Result.
4.7 EXAMPLES
4.7.1 Hexagonal Screw
 Create a new file and save it as Impeller_hexa-bolt.prt
 Choose Insert →Design Feature →
Cylinder
 The cylinder should be pointing in the
Positive ZC-Direction with the center
set at the Origin and with the following
dimensions:
Diameter = 0.25 inches
Height = 1.5 inches
Now create a small step cylinder on top of the
existing cylinder.
 Create a Cylinder with the following dimensions:
Diameter = 0.387 inches
Height = 0.0156 inches
 Click on the top face of the existing cylinder
 On
the
Point
Constructor
window,
choose
the
Arc/Ellipse/Sphere Center icon from the drop-down Type menu
 Click OK to close the Point Constructor window
 Under the Boolean drop-down menu, choose Unite
The two cylinders should look like the figure shown on the right.
 Choose Insert →Curve →Polygon
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 Select the center of the top circle as the Center Point
 On the Sides window, type 6 for the Number of Sides
There are three ways to draw the polygon.
•
Inscribed Radius
•
Circumscribed Radius
•
Side Length
 Choose Side Length and enter the following dimensions:
Length = 0.246 inches
Rotation = 0.00 degree
 Click OK
Now we will extrude this polygon.
 Choose Insert →Design Feature →Extrude
 Choose the Hexagon to be extruded
 Enter the End Distance as 0.1876 inches
The model looks like the following after extrusion.
 On top of the cylinder that has a diameter of 0.387 inches,
insert another cylinder with the following dimensions.
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Diameter = 0.387 inches
Height = 0.1875 inches
You will only be able to see this cylinder when the model is in Static Wireframe since the cylinder
is inside the hexagon head. The model will look like the following.
We will now use the feature operation Intersect.
 Choose Insert →Design Feature →Sphere
 Choose Center Point and Diameter
 Select the bottom of the last cylinder drawn (which is inside the hexagon head and has a
diameter of 0.387 inches and a height of 0.1875 inches) as shown below
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 Give 0.55 as the Diameter
 Choose Intersect in the Boolean dialog box
It will ask you to select the Target Solid
 Choose the hexagonal head
 Click OK
This will give you the hexagonal bolt as shown. Now
we will add Threading to the hexagonal bolt.
 Choose Insert →Design Feature →Thread
 Click on the Detailed radio button
 Keep the Rotation to be Right Hand
 Click on the bolt shaft (the long
cylinder below the hexagon head)
Once the shaft is selected, all the values will
be displayed in the Thread window. Keep all
these default values.
 Click OK
The hexagon bolt should now look like the following.
Save the model.
4.7.2 Hexagonal Nut
 Create
a
new
file
and
save
it
as
Impeller_hexa-nut.prt
 Choose Insert →Curve →Polygon
 Input Number of Dides to be 6
 Create a hexagon with each side measuring 0.28685 inches and constructed at the Origin
 Choose Insert →Design Feature →Extrude
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 Select the Hexagon to be extruded and enter
the End Distance as 0.125 inches
The figure of the model is shown.
 Choose Insert →Design Feature →Sphere
 Enter the Center Point location in the Point
Dialog window as follows
XC = 0; YC = 0; ZC = 0.125
 Enter the Diameter value 0.57 inches
 In the Boolean operations dialog box select
Intersect and click OK
The model will look like the following. We will now
use a Mirror command to create the other side of the
Nut.
 Choose Edit →Transform
 Select the model and click OK
 Click Mirror Through a Plane
 Click on the flat side of the model as shown. Be careful not to select any edges
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 Click on OK
 Click on Copy
 Click Cancel
You will get the following model.
 Choose Insert →Combine Bodies →Unite
 Select the two halves and Unite them
 Insert a Cylinder with the vector pointing in the ZC-Direction and with the following
dimensions:
Diameter = 0.25 inches
Height = 1 inch
 Put the cylinder on the Origin and Subtract this cylinder
from the hexagonal nut
Now, we will chamfer the inside edges of the nut.
 Choose Insert →Detail Feature →Chamfer
 Select the two inner edges as shown and click OK
 Enter the Distance as 0.0436 inches and click OK
You will see the chamfer on the nut. Save the model.
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4.7.3 L-Bar
Here, we will make use of some Primitives and Feature Operations such as Edge Blend, Chamfer,
and Subtract. It should be noted that the same model can be more easily created by 2D Sketching
and Extruding, but Primitives are used here to familiarize the users with these features.
 Create a new file and save it as Arborpress_L-bar
 Choose Insert →Design Feature →Block
 Create a Block with the following dimensions:
Length = 65 inches
Width = 65 inches
Height = 285 inches
 Create the block at the Origin
 Create a second block also placed at the origin with the following
dimensions:
Length = 182 inches
Width = 65 inches
Height = 85 inches
We have to move the second block to the top of the first block:
 Click Edit →Move Object
 Select the second block (green) and click OK
 Choose the Motion as Distance
 Select the positive ZC in the Specify Vector dialog
 Enter 200 as the Distance value
 Make sure that Move Original button is checked and click OK
 Click Move and then Cancel on the next window so that the
operation is not repeated
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Now we will create a Hole. There are several ways to create a Hole. We will do so by first creating
a cylinder and then using the Subtract function.
 Choose Insert →Design Feature
→Cylinder
 On the Specify Vector, select the
YC Axis icon
 In the Specify Point, enter the
following values:
XC = 130
YC = -5
ZC = 242
 The cylinder should have the
following dimensions:
Diameter = 35 inches
Height = 100 inches
 Under the Boolean drop-down window, choose Subtract
 Select the horizontal block at the top
The hole should look like the one in the figure. Now we will create another
cylinder and subtract it from the upper block.
The cylinder should be pointing in the positive Y-direction set at the
following point: XC = 130; YC = 22.5 and ZC = 242 and should have the
following dimensions: Diameter = 66 inches; Height = 20 inches
 Subtract this cylinder from the same block as before using the
Boolean drop-down menu
Now we will create a block.
 Choose Insert →Design Feature →Block
 Create a block with the following dimensions:
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Length = 25 inches
Width = 20 inches
Height = 150 inches
 Click on the Point Dialog icon in the Origin box and enter the
following values:
XC = 157; YC = 22.5; ZC = 180
The model will look like the following figure. Now we will subtract this
block from the block with the hole.
 Choose Insert →Combine Bodies →Subtract
 Click on the block with the two holes (green) as the Target
 Select the newly created block as Tool
 Click OK
The model will be seen as shown. Now we will use the Blend function in
the Feature Operations. We must first unite the two blocks.
 Choose Insert →Combine Bodies →Unite
 Click on the two blocks and click OK
The two blocks are now combined into one solid model.
 Choose Insert →Detail Feature →Edge Blend
 Change the Radius to 60
 Select the edge at the
interface of the two blocks
 Click OK
Repeat the same procedure to Blend
the inner edge of the blocks. This
time, the Radius should be changed
to 30.
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We will now make four holes in the model. You can create these holes by using the Hole option.
However, to practice using Feature Operations, we will subtract cylinders from the block.
 Insert four cylinders individually. They should be pointing in the positive XC-direction
and have the following dimensions.
Diameter = 8 inches
Height = 20 inches
 Construct them in the XC-direction at the following point coordinates:
Cylinder #1: X = 162; Y = 11.25; Z = 210
Cylinder #2: X = 162; Y = 11.25; Z = 275
Cylinder #3: X = 162; Y = 53.75; Z = 210
Cylinder #4: X = 162; Y = 53.75; Z = 275
 Subtract these cylinders from the block in the Boolean dialog
box
The last operation on this model is to create a block and subtract it from
the top block.
 Create a Block with the following dimensions:
Length = 60 inches
Width = 20 inches
Height = 66 inches
 Enter the following values in the Point Dialog as the Origin of
the Block
XC = 130
YC = 22.5
ZC = 209.5
 After creating the block, subtract this block from the block at
the top
The final figure will look like this. Save and close the file.
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4.7.4 Rack
 Create a new part file and save it as Arborpress_rack.prt
 Right-click, then choose Orient View →Isometric
 Choose Insert →Curve →Rectangle
The Point window will open. Note the Cue Line instructions. The Cue Line provides the step that
needs to be taken next. You need to define the corner points for the Rectangle.
For Corner Point 1,
 Type in the coordinates XC = 0, YC = 0, ZC = 0 and click OK
Another Point Constructor window will pop up, allowing you to define the 2nd Corner Point
 Type in the coordinates XC = 240, YC = 25, ZC = 0
and click OK and then Cancel
 Right-click on the screen and choose FIT
Note: We have three options for creating a rectangle:
•
Two point
•
Three points
•
By center
The default option is By 2 Points.
 Choose Insert →Design Feature →Extrude
OR
 Click on the Extrude icon on the Form Feature toolbar.
The Extrude dialog box will pop up.
 Click on the Rectangle.
 Choose the default Positive ZC-direction as the Direction
 In the Limits window, type in the following values:
Start = 0
End = 20
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 Click OK
The extruded body will appear as shown below.
 Choose Insert →Design Feature →
Pocket
 Choose Rectangular in the pop up
window
 Click on the top surface of the rack
 Click on the edge as shown in the figure
for the Horizontal Reference
This will pop up the parameters window.
 Enter the values of parameters as shown
in the figure and choose OK
 When the Positioning window pops up,
choose the PERPENDICULAR option
 Click on the edge of the solid and then
click on the blue dotted line as shown
below
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 Enter the Expression value as 37.8 and Choose OK
 Once again pick the Perpendicular option and then
choose the other set of the edges along the Y-Axis, as
shown on the right (the one perpendicular to the last blue
line selected)
 Enter the expression value as 10 and click OK
 Click OK and then Cancel
The model will now look as follows.
Let us create the instances of the slot as the teeth of the Rack to
be meshed with Pinion.
 Click on Pattern Feature icon in the Feature Group
 Click on the pocket created
 Select Layout as Linear
 Specify vector as positive XC direction
 Choose Count and Pitch in Spacing option and enter value for Count as 19 and that for
Pitch Distance as 9.4
 Click OK
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The model of the Rack will look as the one shown in the figure.
We will now create a Hole at the center of the rectangular cross section. To determine the center
of the cross-section of the rectangular rack, we make use of the Snap Points
 Choose Insert →Design Feature →Cylinder
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 Choose –XC-Direction in the Specify Vector dialog box
 Click on the Point Dialog
 In the Points dialog box select Between Two Points option and select
the points as shown in the figure on the right (diagonally opposite
points). The option selects the midpoint of the face for us
 Click OK
 Enter the following values in the Dimension dialog box
Diameter = 10 inches
Height = 20 inches
 Choose Subtract in the Boolean dialog box
The final model is shown below. Save and close the model.
4.7.5 Impeller
Open the Impeller_impeller.prt file you made in Section 3. It should like the figure below.
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Now let us model a cone.
 Choose Insert →Design Feature →Cone
 Select Diameters and Height
 Select the –XC-Direction in the Specify Vector
dialog box
 In the Point Dialog, enter the coordinates (14, 0, 0).
 Enter the following dimensions:
Base Diameter = 15 inches
Top Diameter = 8 inches
Height = 16.25 inches
The cone will be seen as shown below if you choose Static
Wireframe View.
 Extrude the Airfoil curve in the Z-direction by 12
inches
 Unite the two solids in the Boolean operation dialog
box
The model will be as follows.
Now let us create five instances of this blade to make the
impeller blades.
 Click on Insert →Associative Copy →Pattern
Feature
 Select the Airfoil you just created
 Select Circular layout
 Select the XC-Direction for the Specify Vector and
the Origin for the Specify Point
 For Count, type in 5 and for Pitch Angle, enter 72
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 Click OK
Now, let us create two holes in the cone for the shaft and the locking pin. Note that these holes can
also be created by Hole menu option.
 Subtract a cylinder with a Diameter of 4 inches and a Height of 16 inches from the side
of the cone with the larger diameter
 Subtract another cylinder with a Diameter of 0.275 inches and a Height of 0.25 inches
from the side of the cone with the
smaller diameter
The final model will look like the following.
Save and close your work.
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4.8 STANDARD PARTS LIBRARY
A better and faster approach for modeling standard parts like bolts, nuts, pins, screws, and washers
is using the Standard Parts Library. For example, to model a hexagonal bolt,
 Choose Reuse Library →Reuse Examples →Standard Parts →ANSI Inch →Bolt
 Right-click on Hex Head
 Click on Open Source Folder
 Open Hex Bolt, AI.prt
You can now go to Part Navigator to see all
the steps taken toward modeling this part
and modify any feature. For example to
modify the length of the bolt, right-click on
Extrude (8) “BODY_EXTRUDE” and
choose Edit Parameters.
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4.9 SYNCHRONOUS TECHNOLOGY
One of the important and unique features which NX offers apart from Design Features and
Freeform Modeling is Synchronous Technology. With the options available in Synchronous
Modeling group in the ribbon bar in the Modeling Application tab, the user can modify complex
3D models without the model history tree and without knowing the feature relationships and
dependencies. The “push-and-pull” options can be used to modify the 3D model using faces, edges
and cross-sections. NX 10 supports the Synchronous Modeling to work with 3D models from
CATIA, Pro/ENGINEER®, SolidWorks®, and Autodesk Inventor®, apart from the standard
formats including IGES, ISO/STEP and JT.
For the purpose of illustrating the options available in Synchronous Modeling, let us consider the
impeller part modeled in the previous section and export it as standard STEP format and save it.
 Open a new file in NX
 Choose File →Import →Impeller_impeller.stp
Observe here that the .stp file would not have any model history.
We will explore some of the options available in the Synchronous
Modeling group in the ribbon bar. Click More to view a
comprehensive list of options available in synchronous modeling.
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 Click Delete Face and select the faces of the blade to delete the blade
 Repeat the process and delete all except one blade. The part should look as shown below.
 Click Replace Face and select the end face of the blade with large blend radius as Face to
Replace and select the flat surface of the cone with smaller diameter as the Replacement
Face to delete the blade.
The part should look as shown below.
 Click Move Face and select one side of the blade and enter distance -30 and angle 20 in
the transform section
 Click Resize Blend and select the blended surface of the blade and enter radius as 7 mm
to sharpen the end
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 Click Offset Edge and select the top edge of the blade and choose the method along face
and enter -5 mm in the distance to offset the top surface of the blade
 Click Pattern Face and select four surfaces of the blade and choose Circular Layout and
specify the conical axis as vector, center of the flat surface of the cone as point, count as 6
and pitch angle as 60 radius to pattern six blades.
Therefore, it can be observed that a standard .stp file has been modified by increasing the number
of blades and changing the blade profile. Similarly, the user can either modify any supported 3D
model depending on the design need or create a new 3D model with synchronous modeling “push
and pull” tools.
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4.10 EXERCISES
4.10.1 Circular Base
Model a circle base as shown below using the following dimensions:
Outer diameter = 120 inches
Distance of 3 small slots = 17 inches
Distance of the large slot = 30 inches
Diameter of the central rod = 4 inches and length = 30 inches
Length of slots may vary.
4.10.2 Impeller Upper Casing
Model the upper casing of the Impeller as shown below.
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The dimensions of the upper casing are the same as for the lower casing, which is described in the
previous exercise in detail. The dimensions for the manhole should be such that impeller blades
can be seen and a hand can fit inside to clean the impeller.
4.10.3 Die-Cavity
Model the following part to be used for the Chapter 9 Manufacturing Module. Create a new file
Die_cavity.prt with units in mm not in inches. Create a rectangular Block of 150, 100, 40 along X,
Y and Z, respectively with the point construction value of (-75,-50,-80) about XC, YC and ZC.
Create and Unite another block over the first one with 100, 80 and 40 along X, Y and Z and centrally
located to the previous block.
Create a sketch as shown below including the spline curve and add an Axis line. Dotted lines are
reference lines. While sketching, create them as normal curves. Then right click on the curves and
click convert to reference. Give all the constraints and dimensions as shown in the figure below.
Revolve the curves about the dashed axis as shown above, and subtract the cut with start angle and
end angle as -45 and 45.
Subtract a block of 70, 50, and 30 to create a huge cavity at the centre. Create and Unite 4 cylinders
at the inner corners of the cavity with 20 inches diameter and 15 inches height.
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Add edge blends at the corners as shown in the final Model below. Keep the value of blend as 10
radii for outer edges and 5mm radii for the inner edges.
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CHAPTER 5 – DRAFTING
The NX 10 Drafting application lets you create drawings, views, geometry, dimensions, and
drafting annotations necessary for the completion as well as understanding of an industrial
drawing. The goal of this chapter is to give the designer/draftsman enough knowledge of drafting
tools to create a basic drawing of their design. The drafting application supports the drafting of
engineering models in accordance with ANSI standards. After explaining the basics of the drafting
application, we will go through a step-by-step approach for drafting some of the models created
earlier.
5.1 OVERVIEW
The Drafting Application is designed to allow you produce and maintain industry standard
engineering drawings directly from the 3D model or assembly part. Drawings created in the
Drafting application are fully associative to the model and any changes made to the model are
automatically reflected in the drawing. The Drafting application also offers a set of 2D drawing
tools for 2D centric design and layout requirements. You can produce standalone 2D drawings.
The Drafting Application is based on creating views from a solid model as illustrated below.
Drafting makes it easy to create drawings with orthographic views, section views, imported view,
auxiliary views, dimensions and other annotations.
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Some of the useful features of the Drafting Application are:
1) After you choose the first view, the other orthographic views can be added and aligned
with the click of a few buttons.
2) Each view is associated directly with the solid. Thus, when the solid is changed, the
drawing will be updated directly along with the views and dimensions.
3) Drafting annotations (dimensions, labels, and symbols with leaders) are placed directly on
the drawing and updated automatically when the solid is changed.
We will see how views are created and annotations are used and modified in the step-by-step
examples.
5.2 CREATING A DRAFTING
 Open the file Arborpress_rack.prt
 From the NX 10 Interface, choose File →Drafting as shown or choose Application tab
and select Drafting
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When you first open the Drafting Application, a window pops up asking for inputs like the
Template, Standard Size or Custom Size, the units, and the angle of projection.
Size
Size allows you to choose the size of the Sheet. There are
standard Templates that you can create for frequent use
depending upon the company standards. There are several
Standard sized Sheets available for you. You can also define
a Custom sized sheet in case your drawings do not fit into a
standard sized sheet.
Preview
This shows the overall design of the Template.
Units
Units follow the default units of the parent 3-D model. In case
you are starting from the Drafting Application you need to
choose the units here.
Projection
You can choose the Projection Method either First Angle or
Third Angle method.
To start using the Drafting Application we will begin by
creating a Standard Sized sheet:
 Click on the Standard Size radio button
 In the drop-down menu on the Size window, select
sheet B, which has dimensions 11 x 17
 Change the Scale to 1:25 by using the drop-down
menu and choosing the Custom Scale under the Scale
 Click OK
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This will open the Drafting Application and the following screen will be seen as below. Let us first
look at the Drafting Application Interface.
You will see a dialog box pops-up which will help you choose the parts, views and other options.
 Change the options and views and click Finish
 Choose Insert →View →Base or click on Base
View in the View Group
The Base View dialog box with the options of the View and the Scale will show up along with a
floating drawing of the object.
 Choose the View to be Front
You can find the Front View projection on the screen. You can move the mouse cursor on the
screen and click on the place where you want the view.
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Once you set the Front View another dialog box will pop-up asking you to set the other views at
any location on the screen within the Sheet Boundary.
You can find different views by moving the cursor
around the first view. If you want to add any
orthographic views after closing this file or changing to
other command modes
 Choose Insert →View →Projected View or
choose Projected View
icon from the View
group
Now, let us create all the other orthographic projected
views and click on the screen at the desired position.
 In case you have closed the Projected View dialog box you can reopen it by clicking on
the Projected View icon in the View Group
 Move the cursor and click to get the other views
 Click Close on the Projected View dialog box or press <Esc> key on the keyboard to close
the window
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Before creating the dimensions, let us remove the borders in each view as it adds to the confusion
with the entity lines.
 Choose Menu →Preferences →Drafting or click on
icon in the Quick Access toolbar to find the Drafting
Preferences
The Drafting Preferences window will pop up.
 Click on the VIEW tab button
 Uncheck the Tick mark on the Display Borders as shown in the figure below and click
OK
There are many other options like number of decimal places, hidden lines, angles, and threads that
you can find here. For example, you can find options for hidden lines in Drafting Preferences →
View →Common →Hidden Lines
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5.3 DIMENSIONING
Now we have to create the dimensions for these views. The dimensions can be inserted by either
of the two ways as described below:
 Choose Menu →Insert →Dimension
OR
 Click on the Dimension Toolbar as shown in the following figure
 Click on Points and Edges, move the mouse and click on the appropriate location to draw
dimensions
The icons in this window are helpful for changing the
properties of the dimensions.
 Click on the Settings Button
Here you will be able to modify the settings for
dimensioning. A dialog appears as shown below.
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The first list is for Lettering. This allows the user to justify and select the frame size. In the
Line/Arrow section, you can vary the thickness of the arrow line, arrow head, angle format etc.
The most important section is the Tolerance list. Here you can vary the tolerance to the designed
value.
The type of display, precision required for the digits and other similar options can be modified
here. The next icon is the Text option, which you can use to edit the units, text style, font and other
text related aspects.
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 On the first view (Front View) that you created, click on the top left corner of the rack and
then on the top right corner
The dimension that represents the distance between these points will appear. You can put the
location of the dimension by moving the mouse on the screen. Whenever you place your views in
the Sheet take into consideration that you will be placing the dimensions around it.
 To set the dimension onto the drawing sheet, place the dimension well above the view as
shown and click the left mouse button
Even after creating the dimension, you can edit the properties of the dimensions.
 Right-click on the dimension you just created and choose Settings or Edit Display
 You can modify font, color, style and other finer details here
 Give dimensions to all other views as shown in the following figure
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5.4 SECTIONAL VIEW
Let us create a Sectional View for the same part to show the depth and profile of the hole.
 Choose Insert →View →Section or click the View Section icon
from the View group
in the ribbon bar
 Click on the bottom of the Base View as shown in the figure. This will show a Phantom
Line with two Arrow marks for the direction of the Section plane (orange dashed line with
arrows pointing upwards).
 Click on the middle of the View as shown. This will fix the position of the sectional line
(Section Plane)
Now move the cursor around the view to get the direction of the Plane of Section. Keep the arrow
pointing vertically upwards and drag the sectional view to the bottom of the Base View.
Adjust the positions of dimensions if they are interfering. The final drawing sheet should look like
the one shown in the following figure.
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Save and close your model.
5.5 PRODUCT AND MANUFACTURING INFORMATION
Product and Manufacturing Information (PMI) is one of the important applications in NX which
provides annotation tools used to document products in a 3D environment. PMI application
includes a comprehensive 3D annotation environment that allows design teams to share details
such as Geometric Dimensioning and Tolerancing (GD&T), surface finish, welding information,
material specifications, comments, government security information or proprietary information,
etc. directly to the 3D model. PMI complies with industry standards for 3D product definition and
therefore product teams working on collaborative projects would use 3D models as a legitimate
method for fully documenting product and manufacturing information.
In the below example, we will open a part file, create dimensions and comments on the 3D model
in the PMI application and learn how to inherit the dimensions and comments to the Drafting
application. This is only for the purpose of illustration.
 Open the file Impeller_impeller.prt
 From the NX 10 interface, choose File →PMI (turn on the check mark)
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This should create an additional tab PMI in between Tools and Application tabs. Select the PMI
tab to enter the PMI application which should look as shown below.
The ribbon bar in this mode would have the Dimension, Annotation, Custom Symbols,
Supplemental Geometry, Specialized and Security Marking groups. Each group has several options
which could help describe the modeled 3D part. For example, dimensioning options in Dimension
group, Surface Finish and Notes in Annotation group.
 Click Rapid icon
 Select the end surfaces of the impeller as first and second objects to insert the linear
dimension or click the Linear icon to perform the same task
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 Click the Radial icon in the Dimension group to insert the dimensions of the holes and
curved surfaces on the impeller
 Click the Centerline icon
in the Supplemental Geometry group and select the
inner surface of the impeller to insert the centerline for the part
 Click the Note icon in Annotation group to provide any comments or Surface Finish icon,
select the object, location of text and leader line to insert the specific surface finish details,
if required
The Trimetric view of the impeller after PMI dimensioning would look as shown below.
 Save the file, select Application tab and click on Drafting icon in the ribbon bar
 Follow the similar procedures explained in the previous section to create the Drawing sheet
for the 3D part
During the creation of the sheet, in the View Creation Wizard, select the Inherit PMI option, and
select the Aligned to Drawing (Entire Part) and check the Inherit PMI onto Drawing option. This
would inherit the dimensions of the 3D model and show on the drawing sheet including the
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comments as shown below. The user has to select the appropriate views to reflect the dimensions
on the drawing sheet.
5.6 EXAMPLE
 Open the model Impeller_hexa-bolt.prt
 Choose File →Drafting or select Drafting in Application tab
 On the Sheet window, select sheet E-34 X 44 and change the Scale value to 8.0 : 1.0
 Click OK
 Choose Insert →View →Base View or click the Base View icon
 Add the Front view by repeating the same
procedure explained in the last example
 Add the Orthographic Views including the Right
view and Top view
 Choose Preferences →Drafting
 Uncheck the box next to Display Borders under
View Tab
The screen will have the following three views.
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To see the hidden lines,
 Choose Preferences →Drafting →View
OR
 Select the views, right-click and choose Settings as shown below
A window will pop up with various options pertaining to the views.
 Click on the Hidden Lines tab
 Change Process Hidden Lines to Dashed Lines as shown below and click OK
You can see the hidden lines as shown in the
picture on the right.
Now we will proceed to dimensioning.
 Choose Insert →Dimensions →Linear or
click the Linear Dimension icon
in the
Dimension group
 Give vertical dimensions to all the
distances shown below
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For the threading, we will use a leader line.
 Click on the Note icon shown in the Toolbar
 In the Note window that opens, enter the following
text. You can find Ø and the degree symbol on the
Symbols tab
Right Hand Ø 0.20 x 1.5
Pitch 0.05, Angle 600
 Click on the threaded shaft in the side view, hold
the mouse and drag the Leader line next to the
view. Let go of the mouse and click again to place
the text.
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 Close the Annotation Editor
Since the height of the Lettering is small, we will enlarge the character size as well as the arrow
size.
 Right-click on the Leader and select Settings
 Click on the Lettering tab
 In the Text Parameter section, increase Height to make the leader legible
 Click on the Line/Arrow tab
 In the Format section, increase the Length of the Leader
Now we will add additional dimensions and views.
 Choose Insert →Dimensions →Radial or click the Radial Dimension icon
in the
Dimension group
 Click the circle of the bolt in the top view to give the diameter dimension
 Click Insert →View →Base View of click the Base View icon
 Select the Isometric view and place the view somewhere on the screen
The final drawing is shown below. Remember to save.
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5.7 EXERCISE
Perform Drafting and give dimensions to the circle base that you modeled in Exercise 4.8.1.
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CHAPTER 6 – ASSEMBLY MODELING
Every day, we see many examples of components that are assembled together into one model such
as bicycles, cars, and computers. All of these products were created by designing and
manufacturing individual parts and then fitting them together. The designers who create them have
to carefully plan each part so that they all fit together perfectly in order to perform the desired
function.
In this chapter, you will learn two kinds of approaches used in Assembly modeling. We will
practice assembly modeling using the impeller assembly as an example. Some parts of this
assembly have already been modeled in earlier chapters.
NX 10 Assembly is a part file that contains the individual parts. They are added to the part file in
such a way that the parts are virtually in the assembly and linked to the original part. This
eliminates the need for creating separate memory space for the individual parts in the computer.
All the parts are selectable and can be used in the design process for information and mating to
insure a perfect fit as intended by the designers. The following figure is a schematic, which shows
how components are added to make an assembly.
6.1 TERMINOLOGY
Assembly
An assembly is a collection of pointers to piece parts and/or subassemblies. An assembly is a part
file, which contains component objects.
Component Object
A component object is a non-geometric pointer to the part file that contains the component
geometry. Component object stores information such as the Layer, Color, Reference set, position
data for component relative to assembly and path of the component part on file system.
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Component Part
A component part is a part file pointed to by
a component object within an assembly. The
actual geometry is stored in the component
part and is referenced, not copied by the
assembly.
Component Occurrences
An occurrence of a component is a pointer to geometry in the component file. Use component
occurrences to create one or more references to a component without creating additional geometry.
Reference Set
A reference set is a named collection of objects in a component part or subassembly that you can
use to simplify the representation of the component part in higher level assemblies.
6.2 ASSEMBLING APPROACHES
There are two basic ways of creating any assembly model.
•
Top-Down Approach
•
Bottom-Up Approach
6.2.1 Top-Down Approach
In this approach, the assembly part file is created
first and components are created in that file. Then
individual parts are modeled. This type of
modeling is useful in a new design.
6.2.2 Bottom-Up Approach
The component parts are created first in the
traditional way and then added to the assembly
part file. This technique is particularly useful,
when part files already exist from the previous
designs, and can be reused.
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6.2.3 Mixing and Matching
You can combine these two approaches, when
necessary, to add flexibility to your assembly
design needs.
6.3 ASSEMBLY NAVIGATOR
The Assembly Navigator is located on top of the
Part Navigator in the Resource Bar on the left of
the screen. The navigator shows you various things
that form the assembly, including part hierarchy,
the part name, information regarding the part such
as whether the part is read only, the position, which
lets you know whether the part is constrained using
assembly constraints or mating condition, and the reference set. Following is a list of interpretation
of the Position of the components.
Indicates a fully constrained component
Indicates a fully mated component
(Fixed) Indicates that all the degrees of freedom are constrained
Indicates partially constrained component
Indicates partially mated component
Indicates that the component is not constrained or mated
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6.4 MATING CONSTRAINTS
After the Component Objects are added to the assembly part file, each Component Object is mated
with the existing objects. By assigning the mating conditions on components of an assembly, you
establish positional relationships, or constraints, among those components. These relationships are
termed Mating Constraints. A mating condition is made up of one or more mating constraints.
There are different mating constraints as explained below:
Touch/Align: Planar objects selected to align will be coplanar but the normals to the planes
will point in the same direction. Centerlines of cylindrical objects will be in line with each
other.
Concentric: Constrains circular or elliptical edges of two components so the centers are
coincident and the planes of the edges are coplanar.
Distance: This establishes a +/- distance (offset) value between two objects
Parallel: Objects selected will be parallel to each other.
Perpendicular: Objects selected will be perpendicular to each other.
Bond: Creates a weld and welds components together to move as single object.
Center: Objects will be centered between other objects, i.e. locating a cylinder along a slot
and centering the cylinder in the slot.
Angle: This fixes a constant angle between the two object entities chosen on the components
to be assembled.
6.5 EXAMPLE
We will assemble the impeller component objects. You have modeled all the components in
previous chapters. Now we have to insert them into the assembly environment and apply
constraints to locate them relative to each other. Once the assembling is completed, we can create
an exploded view and prepare the drafting.
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Before starting the assembly modeling, make two through-holes on each side of the Impellerlower-casing and Impeller-upper-casing (a total number of 4 holes for each casing) for the Hexabolt. Diameter of the holes should be 0.25 and their location should be similar to the figure below.
Make sure to create the holes in the same places for lower and upper casing to that when they are
assembled they match.
6.5.1 Starting an Assembly
 Create a new file
 Choose Assembly under the Model tab
 Name it as Impeller_assembly.prt
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OR, if you are in the Modeling Application and want to start assembling,
 Turn on Assemblies option in Application tab and a new Assemblies tab shows up
OR
 Click File →Assemblies as shown below
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 The Home menu bar will now display tools for assembly
In the Components option,
•
Add option adds new component objects whose part files are already present.
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•
Create New lets you create new component geometries inside the assembly file in case you
are using Top-Down approach of assembly.
The Assembly Constraints allows you to create assembly constraints and Move Components allows
you to reposition the components wherever you want them in the assembly.
6.5.2 Adding Components and Constraints
 Choose Add
The dialogue box on the right side will pop up. You can select the part files from those existing
(should be already shown in Loaded Parts tab) or you can load
the part files using the Open file options in the dialog box. This
will load the selected part file into the Loaded Parts dialog box.
 Click on the Open icon and select the file
Impeller_upper-casing.prt
 Click OK in the part name dialog box
You will see that a small copy of the component object appears
in a separate window on the screen as shown in the figure
below.
You will need to place this figure initially at a certain location. This can be done by changing the
Positioning option in the Placement dialog box to Absolute Origin.
 Click OK
Now we will add the second component, the lower casing.
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 Click on Add in the assembly section
 Select the file Impeller_lower-casing.prt
 In the Poistioning dialog box change the option to By Constraints
 Choose Apply
This will show you the added component in a Component
Preview window as before.
Now let us mate the upper and the lower casing. You can
access all the constraints in the drop-down menu in the
Type dialog box in the Assembly Constraints menu. The
following dialog box will appear.
Here you can see the different Mating Types, which were
explained above in the previous section.
 Make sure the Touch Align icon
is selected
in the Type dialog box
 First, select the face that the arrow is pointing to in
the Component Preview window as shown below
in the figure on the left.
 Click on the face of the upper casing in the main screen as shown in the figure on the right.
You may have to rotate the figure in order to select the faces.
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 Click on the Assembly Constraints
 Choose the Touch Align as the Type
 Click on the Flange of the lower casing
 Click on the Flange of the upper casing, you may need to inverse the direction of constraint
by click on the Inverse icon
Note: if it is difficult for you to select the faces because of the position of the parts, you can move
them by clicking on the Move Component in the same Assemblies group.
 Select the Tough Align again
 Click on the flat face of the lower casing as shown and then the same face on the upper
casing
The two assembled components will be seen as shown in the figure below.
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The lower casing is constrained with respect to the upper casing. Now let us add the impeller.
 Choose Assemblies →Components →Add Component as an alternative way to add a
component to the assmbly
 Open the file Impeller_impeller.prt
 Click OK on the dialog box
 Click on the Distance icon
in the Type dialog box
 Select the two faces, first on the impeller and then on the casing, as shown in the figure
below
 Click OK
 In the Distance dialog box in the Assembly
Constraints window, enter a value of 3
 On the Assembly Constraints window,
uncheck the Preview Window option
The preview may show the impeller oriented in the
direction opposite to the one we want.
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 On the Assembly Constraints window, click on the Reverse the Last Constraint option
in the Geometry to Constrain
Now the impeller will be oriented in the right direction.
We will now add the shaft using the Center constraint.
 Click on Assemblies →Components →Add
Component
 Open the file Impeller_shaft.prt
 Click OK on the dialog box
 Choose the Touch Align icon
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 Choose the Infer Center/Axis option in the Geometry to Constrain dialog
 Select the two surfaces, first on the shaft in the preview window and then on the impeller
on the main screen as shown in the figures below
 Choose the Touch Align
constraint
 First, select the face on the shaft and then select the bottom face of the hole in the impeller
as shown
 Choose Apply and then click OK
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The assembly will now look like the figure below.
 Click on Assemblies →Components →Add Component
 Open the file Impeller_hexa-bolt.prt
 Choose the Touch Align constraint. Use the Infer Center/Axis option in the Geometry
to Constrain dialog box
 First, select the outer cylindrical threading on the bolt and then select the inner surface of
the hole on the upper casing as show in the figures below.
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 Again in the Touch Align constraint change the Geometry to Constrain option to Prefer
Touch
 Select the flat face on the bolt and the face on the rib of the upper casing as shown
 Click Apply and then OK
The assembly is shown below.
 Repeat the same procedure to add bolts and nuts to all the holes in the casing.
This completes the assembly of the impeller.
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Note: There is a simpler way to assemble the bolt and nut set. Instead of adding the three parts
individually, you can assemble these components separately in another file. This will be a subassembly. You can insert this subassembly and mate it with the main assembly.
The Final Assembly will look as the shown below. Save the Model.
6.5.3 Exploded View
In this section, we are going to create an Exploded View of the assembly to show a separated partby-part picture of the components that make the assembly. In today’s industrial practice, these
kind of views are very helpful on the assembly shop floor to get a good idea of which item fixes
where. The user should understand that exploding an assembly does not mean relocation of the
components, but only viewing the models in the form of disassembly. You can Unexplode the view
at any time you want to regain the original assembly view. Let us explode the Impeller Assembly.
 Choose Menu →Assemblies →Exploded Views →New Explosion
This will pop a dialog box asking for the name of the
Explosion view to be created. You can leave name as
the default name and choose OK
Now the NX environment is in Exploded View
environment though you do not find any difference. When we start exploding an assembly, we
should decide upon a component to keep that component as the reference. This component should
not be moved from its original position. In the case of the impeller assembly, the impeller will be
the right option as it is central to the entire assembly. Now let us start exploding the components.
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 Right click on the upper casing and choose Edit Explosion
The Edit Explosion window will pop up along with a coordinate system on the component.
 Click on the Z axis; hold the mouse and drag upwards until the reading in the Distance
shows -20 (substitute +20 if you have designed in opposite direction)
 Click OK
 Right click on the lower casing and choose Edit
Explosion
Again, this will pop up a dialog window for Edit
Explosion and a coordinate system on the component.
 Click on the Z-axis; hold the mouse and drag
downwards until the reading in the Distance
shows 20 as shown in the following figure.
 Right click on the shaft and choose Edit
Explosion
 This time click on the X-axis; hold the button and drag to the right side until the reading in
the distance shows -25 as shown in the following figure
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 Choose OK
 Select all the four hexagonal bolts in the assembly by clicking on them
 Right click on one of them and choose Edit Explosion
 This time click on the Z-axis; hold the button and drag upwards until the reading in the
Distance shows 25 as shown in the following figure. This will move all the six bolts
together to the same distance.
 Choose OK
 Likewise, select all the four hexagonal nuts together and move them downwards to a value
of -30.
This is the Exploded view of the assembly. You can rotate and see how it looks like.
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If you want to retain the original assembly view you can Unexplode any component,
 Right click on the component and choose Unexplode.
If you want to unexplode all the components,
 Choose Assemblies → Exploded Views → Unexplode Component
 Select all the components and choose OK
6.6 EXERCISE
In previous sections of this tutorial, we have modeled various parts, some of which are components
of the arbor press, which is shown below. Assemble the arbor press using the components that you
have modeled in addition to ones that are provided to you that you have not modeled before. The
complete list of parts that the arbor press assembly consists of includes:
•
Allen Bolt
•
Allen Nut
•
Base
•
Circle base
•
End clip
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•
Handle
•
Hexagonal Bolt
•
L-bar
•
Pin
•
Pinion
•
Pinion handle
•
Plate
•
Rack
•
Sleeve
All these parts are provided in a folder that can be accessed along with this tutorial in the same
internet address (https://web.mst.edu/~mleu/).
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CHAPTER 7 – FREEFORMING
In this chapter, you will learn how to create freeform models in NX 10. Up to this point, you have
learned different ways to create models by using Form Features or by Sketching. Freeform
modeling involves creating solids in the form of surfaces particularly the B-surface. Because of
their construction techniques and design applications, these surfaces are usually stylistic. A few
freeform features are shown below.
To create Freeform Features, you first need a set of points, curves, edges of sheets or solids, faces
of sheets or solids, or other objects. The following sections cover some of the methods that you
can use to create solids using some of the freeform features.
7.1 OVERVIEW
The Freeform Features in NX 10 are grouped under various menus and located in the INSERT
menu. There are a lot of ways in which you can create Freeform Features from the existing
geometry you have like points, edges, curves, etc. These options are located at various places like
Menu →Insert →Surface/Mesh Surface/Sweep/Flange Surface and Menu →Edit →Surface for
more advanced options A few of the menus that are more useful are discussed below.
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7.1.1 Creating Freeform Features from Points
In the case where the geometry you are constructing or preexisting data includes only points, you may be able to use
one of these three options to build the feature from the
given points.
 Click on Insert →Surface
Four point surface: if you have four corner points.
Through Points: if the points form a rectangular
array.
From Poles: if defined points form a rectangular array
tangential to the lines passing through them.
7.1.2 Creating Freeform Features from Section Strings
If construction geometry contains strings of connected objects (curves and edges), you may be
able to use one of these two options to build the feature.
 Click on Insert →Mesh Surface
Ruled: Used if two strings are roughly parallel.
Through Curves: Used if the three or more strings are
roughly parallel.
If construction geometry contains two or more strings (curves, faces, edges) that are roughly
parallel to each other, and one or more section strings that are roughly perpendicular to the first
set of curves (guides), you may be able to use one of these following options to build the feature.
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Through Curve Mesh: Used if at least four section
strings exist with at least two strings in each direction (parallel
and perpendicular).
Swept: Used if at least two section strings are roughly
perpendicular (choose Insert →Sweep).
7.1.3 Creating Freeform Features from Faces
If the construction geometry contains a sheet or face, you may be able to use one of the following
two options to build the feature.
 Click on Insert →Offset/Scale
Offset Surface: Use this option if you have a face to
offset.
 Click on the Insert →Flnage Surface →Extension
Extension: Use this option if you have a face and edges, edge curves, or curves on the face.
7.2 FREEFORM FEATURE MODELING
Let us do some freeform modeling on structured points, a point cloud, curves and faces. Structured
points are a set of point’s defined rows and columns. A point cloud has a set of scattered points
that form a cloud.
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7.2.1 Modeling with Points
 Open the file freeform_thrupoints.prt
 Right-click on the Toolbars and make sure the Surface Toolbar is checked
You will see seven rows with many points.
 Choose Insert →Surface →Through Points
OR
 Click on the Icon
in the Toolbar
The dialogue box will pop up as shown in the right.
 For Patch Type, select Multiple
 For Closed Along, select Neither
 For Row Degree and Column Degree, enter 3.
 Click OK
The next dialogue box will be as shown.
 Click Chain from All
 Select the top starting point and the bottom ending point of the left most row as shown in
the following figure
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The first row of points will be highlighted.
 Repeat the same procedure to select the first four strings of points.
After that, a window should pop-up asking if all points
are specified or if you want to specify another row.
 Select Specify Another Row until all rows are
specified
 When all the rows are specified, choose All Points Specified
 Click Cancel on the Through Points window
You will see the surface as shown below.
7.2.2 Modeling with a Point Cloud
 Open the file named freeform_throughcloud.prt
The point cloud will be seen as follows.
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 Choose Insert →Surface →Fit Surface
OR
 Click on this icon
on the Surface Toolbar
The following dialogue box will appear.
 Select all the points on the screen by clicking on the
point cloud.
 In the Fit Direction drop-down menu, choose Best Fit
for. This matches the point cloud coordinate system
with original system
 Change the default values for U and V degrees to 3
 Click OK
The final sheet will look like the following.
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7.2.3 Modeling with Curves
 Open the file named freeform_thrucurves_parameter.prt
The curves will be seen as in the figure below.
 Choose Insert →Mesh Surface →Through Curves
OR
 Click on this Icon
on the Toolbar
 Select the first section string as shown below. Be sure to select somewhere on the left side
of the arc.
A direction vector displays at the end of the string.
 Click the middle mouse button MB2
 Click on the next curve similar to first one and click the middle mouse button MB2. You
can see a surface generated between the two curves as shown in the figure
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 Repeat the same procedure to select the remaining strings. Remember to click MB2 after
selecting each curve.
 For Alignment, choose Parameter
 For Patch Type, choose Single
 For Construction, choose Simple
When the Simple option is activated, the system tries to
build the simplest surface possible and minimize the
number of patches.
 Click OK
7.2.4 Modeling with Curves and Faces
 Open
the
file
1
named
2
freeform_thrucurves_faces.prt
The curve and faces will be seen as follows.
 Choose Insert →Mesh Surface →
Through Curves
 Select the left edge of the top plane
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 Select the middle edge and click MB2
 Select the line
 In the Dialog box, under the Alignment section, uncheck the Preserve Shape check box
You would get the following shape displayed on screen.
Make sure that all the arrows are pointing in the same direction.
 In the Alignment dialog box choose Parameter
 In the Continuity dialog box select G2 (Curvature) option and select the two faces of the
top plane as shown
 Click APPLY
 Now select the middle edge and click MB2
 Select the edge of the lower plane and click MB2
 Click MB2 to finish the curve selection
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 Change the option to G2 (Curvature) in the Continuity dialog box
 Select the face of the upper surface(newly created and click MB2
 Select the bottom face
 Click APPLY and then click Cancel
The final curve will be seen as shown below.
7.3 EXERCISE
Model a computer mouse similar to the one shown below or use your imagination to model a
different mouse. As a hint, create some boundary curves on different planes and use them to form
freeform surfaces. Use these quilt surfaces to create the solid. Add and subtract blocks and pads to
attach the accessories like buttons.
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CHAPTER 8 – FINITE ELEMENT ANALYSIS
Finite Element Analysis (FEA) is a method for predicting the response of structures and materials
to environmental factors such as forces, heat and vibration. The process starts with the creation of
a geometric model. The model is then subdivided (meshed) into small pieces (elements) of simple
geometric shapes connected at specific node points. In this manner, the stress-strain relationships
are more easily approximated. Finally, the material behavior and the boundary conditions are
applied to each element. Software such as NX 10 computerizes the process and makes it possible
to solve complex calculations a matter of minutes. It can provide the engineer with deep insights
regarding the behavior of objects.
Some of the applications of FEA are Structural Analysis, Thermal Analysis, Fluid Flow Dynamics,
and Electromagnetic Compatibility. Of these, FEA is most commonly used in structural and solid
mechanics applications for calculating stresses and displacements. These are often critical to the
performance of the hardware and can be used to predict failures. In this chapter, we are going to
deal with the structural stress and strain analysis of solid geometries.
8.1 OVERVIEW
8.1.1 Element Shapes and Nodes
The elements can be classified into different types based on the number of dimensions and the
number of nodes in the element. The following are some of the types of elements used for
discretization.
One-dimensional elements
Two-dimensional elements
Triangular:
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Quadrilateral:
Three-dimensional elements
Tetrahedral (a solid with 4 triangular faces):
Hexahedral (a solid with 6 quadrilateral faces):
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Types of nodes
Corner nodes
Exterior nodes
Side nodes
Interior nodes
The results of FEA should converge to the exact solution as the size of finite element becomes
smaller and smaller.
8.1.2 Solution Steps
Starting the Simulation: You can select the solver algorithm from one of these: NX Nastran, NX
Thermal/Flow, NX Nastran Design, MSC NASTRAN, Ansys, Abaqus, NX Electronic Systems
Cooling, NX Space Systems Thermal, LS-DYNA, and NX Multiphysics. In addition, you can
choose the type of analysis to be performed. In this tutorial, only Structural Analysis will be
covered with NX Nastran Design.
Choosing the Material Properties: This allows you to change the physical properties of the
material that will be used for the model. For example, if we use steel to manufacture the impeller,
we can enter the constants such as density, Poisson’s ratio, etc. These material properties can also
be saved in the library for future use or can be retrieved from Library of Materials.
Applying the Loads: This option allows you to exert different types of forces and pressures to act
on the solid along with the directions and magnitudes.
Applying the Boundary Conditions: Boundary conditions are surfaces that are fixed to arrest the
degrees of freedom. Some surfaces can be rotationally fixed and some can be constrained from
translational movement.
Meshing the Bodies: This is used to discretize the model as discussed in beginning of the chapter.
Normally, we select tetrahedral shapes of elements for approximation. You can still select the 2D and 1-D elements depending on the situation and requirements by choosing these options from
the drop-down menu.
Solution and Results: This is the command to solve all the governing equations by the algorithm
that you choose and all the above options. This solves and gives the result of the analysis of the
scenario.
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8.1.3 Simulation Navigator
The Simulation Navigator provides the capability to activate
existing solutions, create new ones, and use the created solution
to build mechanisms by creating and modifying motion objects.
To display the Simulation Navigator,
 Click the Simulation Navigator tab in the Resource
bar as shown in the figure
It shows the list of the scenarios created for the master model
file. In each scenario, it displays the list of loads, boundary
conditions, types of meshes, results, reports generated and so
on.
8.2 SCENARIO CREATION
 Copy and paste the file Impeller_impeller.prt into a new folder to avoid changes being
made to the assembly
 Click on New →Simulations if the part is NOT already opened in the NX window
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 Open this newly copied file
 If part is already opened in NX, then click on File →Advanced Simulations
The following figure is the toolbar for Finite Element Modeling and Analysis of Structures.
The Design Simulation module is different from when the first scenario is created. NX creates a
folder of the same name as that of the file and at the same location where the file is located. For
every scenario or Solution, it creates five different files with the name of the scenario. They are
xxx.SIM, xxx.DAT, xxx.txt, xxx.out and xxx.VDM. All the results generated for the scenarios are
saved as .VDM files. You can think of a scenario model as a variation of a master design model.
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Scenarios contain all the geometric features of the master model. They also support body
promotions and interpart expressions.
Body promotions are used to provide an independently modifiable copy of the master model
geometry and serve as a place to hold scenario-specific features such as mid-surfaces. The scenario
model's geometry is linked to the master model geometry, but a scenario may have additional
unique information. For example, the master model may contain all the information about the
model's geometry, but the scenario model will contain additional motion data, such as information
about links and joints.
Note: When you first open any file in Design Simulation module, it will automatically pop up with
Solution Creation window to create a solution.
 Click on the New FEM and Simulation icon on the
toolbar
This will pop up the New FEM and Simulation dialog box to
create a new scenario.
 Click OK
This pops up another window that creates different scenarios as
shown below.
In the Solution window, you can select the Solver and the Analysis Type.
The default Solver type is NX Nastran Design and Analysis type as Structural.
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 Choose OK to create a new Solution called Analysis_1, which is displayed in the
Simulation Navigator
The Simulation Navigator will now look like the following figure.
8.3 MATERIAL PROPERTIES
The next step is to give the material properties to the solid model for this scenario. Because we do
not have any data in the library to retrieve for standard material, we will create one. Let us assume
that we will use steel to manufacture the impeller.
 Click on the More icon in Properties group on the Toolbar
 Choose Assign Materials
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The Assign Materials window will pop up. You have
the option of choosing the pre-defined materials
from the Library or create a new material.
 Select the Impeller
 Choose Local Materials
 Click on the Create icon
Enter the name and values as shown in the following
figure. Pay attention to the units.
(Note that 30e6 represents 30×106)
 Choose OK to exit the Isotropic Material
window
This will assign the material properties to the
impeller. Now let us attach the load.
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8.4 MESHING
The Mesh option discretizes the model into
small elements.
 Click on the 3D Tetrahedral Mesh
icon
A window will pop up asking for the type
and size of the elements.
 Click on the solid object model on
the graphic screen.
There are two types of Tetrahedral
Elements available in NX 10. One is 4nodes and the other is 10-node.
 Choose the Type to be TETRA10
 Enter the Overall Element Size as
1.0
 Choose OK
You can find the model with small
tetrahedral elements. It will look like the
figure shown below.
Note: While meshing the solid there is a
trade-off you need to consider. If you
choose a smaller element with higher
nodes you will get better accuracy in your analysis than larger element. However, the time required
to solve the model with smaller elements will much greater than with larger element. Hence, based
on the accuracy requirement of the study and how critical the component is in terms of the end
product choose the appropriate size of the elements and nodes.
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8.5 LOADS
The loads applied on the solid model should be input to the system. For the impeller, the major
force acts on the concave surfaces of the turbine blades. This loading can be approximated by
normal pressure on all the five surfaces. Since we are not concerned about the magnitude of the
load, let us take the value to be 100 lbf/sq inch to exaggerate the deformation of the blades.
 Click on the Activate Simulation to apply loads as shown below
 Click on Load Type and choose Pressure
 Click on the five concave surfaces of the blades as shown in the following figure
 Enter the value for Pressure as 100 and keep the units as lb-f/in2 (psi)
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8.6 BOUNDARY CONDITIONS
The impeller rotates about the axis of the cone with the shaft as you can see in the assembly in the
previous chapters. It is not fixed but our concern is the deformation of the blades with respect to
the core of the impeller. The conical core is relatively fixed and the deformations of the blades are
to be analyzed accordingly.
 Click on the Constraint Type icon
 Select the Fixed Constraint
This type of constraint will restrict the selected entity in six DOF from translating and rotating.
You can see the different constraints available by clicking the Constraint Type drop-down menu
on the toolbar.
 Click on the conical surface of the impeller as shown in the following figure
 Click OK
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8.7 RESULT AND SIMULATION
8.7.1 Solving the Scenario
The Finite Element Model is now ready for solving and analysis. It is a good practice to first check
for model completion before we get into solving the model. To check the model
 Click on the Menu →Analysis →Finite Element Mode Check →Model Setup or click
the Model Setup icon in the Checks and Information group in the ribbon bar
This will pop-up a menu as shown on the right.
 Choose OK
This will display the result of the Check. You will be
able to see any errors and warnings in a separate
window. In case you get errors or warnings go back
to the previous steps and complete the required
things. If you do not get errors or warnings you are
ready to solve the FEA problem.
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 Click on the Solve icon
This will open the Solve window.
 Click OK without making any changes
It may take a while to generate the results. Wait until the
Analysis Job Monitor window appears, showing the job to
be Completed. While the solver is doing computations, the
Analysis Job Monitor will show as Running
 Click on Cancel when the Analysis Job Monitor
window shows Completed
8.7.2 FEA Result
 Click on Open Results
 Click on the Post Processing Navigator
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The Post-Processing Navigator shows all the Solution you created. If you click the ‘+’ sign in
front of the Solution you will see the different analyses that have been performed on the model.
 Double-click on the Displacement-Nodal
menu
The screen will now appear as shown below. You can
easily interpret the results from the color-coding. The
orange-red color shows the maximum deformation
zones and the blue area shows the minimum deformation zones. You can observe that because the
conical core is fixed, it experiences zero deformation. The analysis also shows that the maximum
deformation experienced at the tip of the blades is 1.245 x 10-3 inches.
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On the Post-Processing Navigator, you can keep changing the results by double clicking each
option as shown below. You can click on the other inactive marks to see various results. Some of
the other results are shown below.
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8.7.3 Simulation and Animation
The Post Processing Toolbar should appear when you select the Design Simulation Module.
However, in case it does not become visible follow these steps.
 Click on the Results tab. A group for Animation can be seen on it as follows
 Click on the Animation icon.
 In the Animation window, change the number of
frames to 10 and click on the Play button
to see
the animation of the deformation
You can now see an animation of how the impeller is
deformed as the loads are applied to the blades.
 To make any setting changes in the results display,
click on the Edit Post View icon
 Check the Show undeformed model and click OK
Now press on the Play button to see the animation.
This will show the animation of deformation with
the original shape in grey color, as shown in the
figure below.
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 Click on the Stop button
 Right-click on the Return to Home to go back to the meshed model
There are two ways to improve the accuracy of FEA results.
•
Reduce the size of element
•
Increase the order of interpolation polynomial (i.e. use quadratic or even cubic instead of
linear polynomials)
The second approach is preferred because it is more efficient in terms of computation time and
takes less memory space. However, let us try to create a scenario using the first option.
 Right-click on Solution 1 in the Simulation
Navigator
 Choose Clone to copy the first scenario
 Once Copy of Solution 1 is created, rename it to
Solution 2
 Go to .fem1 file in the Simulation File View
 Right click on the 3D Mesh (1) and click Edit
 In the dialog box shown, change the Type to
TETRA4
 Choose OK
 Go to .sim1 file in the Simulation File View
 Click on the Solve icon
to solve the scenario
 Click OK
The Analysis Job Monitor should show the status of Solution
2 to be Completed.
 Click Cancel
 In the Simulation Navigator, double-click on Results for Solution 2
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The figure below shows the analysis. You can observe the change in the maximum deviation. Save
all the scenarios and close the files.
8.8 EXERCISE
Open the file ‘Arborpress_L-bar.prt’ and do a similar structure
analysis, considering the material as steel. For the mesh, the
element size should be 10.00 and the type Tetra10. For the loads,
apply a normal pressure with a magnitude of 500 on the top surface
as shown in the figure.
For the boundary conditions, fix the three flat faces (the front
highlighted face, the face parallel to it at the backside and the
bottom face) as marked in the following figure.
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CHAPTER 9 – MANUFACTURING
As we discussed in Chapter 1 about the product realization process, the models and drawings
created by the designer have to undergo other processes to get to the finished product. This being
the essence of CAD/CAM integration, the most widely and commonly used technique is to
generate program codes for CNC machines to mill the part. This technological development
reduces the amount of human intervention in creating CNC codes. This also facilitates the
designers to create complex systems. In this chapter, we will cover the Manufacturing Module of
NX 10 to generate CNC codes for 3-Axis Vertical Machining Centers. This module allows you to
program and do some post-processing on drilling, milling, turning and wire-cut EDM tool paths.
9.1 GETTING STARTED
A few preparatory steps need to be performed on every CAD model before moving it into the
CAM environment. Throughout this chapter, we are going to work with one of the models that
were given in the exercise problems. For a change, all the units are followed in millimeters in this
model and manufacturing of the component.
Before getting started, it would be helpful if you can get into a CAM Advanced Role. To do this,
go to the Roles menu on the Resource Bar. A drop-down
menu will pop up in which the CAM Advanced role can
be seen as shown in the figure.
9.1.1 Creation of a Blank
After completing the modeling, you should decide upon
the raw material shape and size that needs to be loaded on
the machine for the actual machining. This data has to be
input in NX 10. This can be achieved in two ways. The
first method is by creating or importing the model of the
raw material as a separate solid in the same file and
assigning that solid as the Blank. The second method is
by letting the software decide the extreme dimensions of
the designed part and some offset values if wanted. The
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later method allows a quick way of assigning the raw size details but it can only be used for
prismatic shapes.
 Open the file Die_cavity.prt of the exercise problem in Chapter 4
 Insert a block with the following dimensions and positioning
Length = 150 mm
Width = 100 mm
Height = 80 mm
 In the Point Constructor icon located on the toolbar choose the lower most edge of the
base block, so that the new block created wraps up the whole previous model as shown
This block encloses the entire design part so we will change the display properties of the block
 Click on the Edit Object Display icon in the Visualization group of the View tab
 Select the block you created and click OK
 When the window pops up, change the display Color and change the Translucency to 50
 click OK
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 Hide the block you just created by right clicking on the block in the Part Navigator. This
will make the raw block disappear from the environment. Whenever you want to view or
work on this solid, reverse the blanks. This is done by pressing <Ctrl> + <Shift> + B.
9.1.2 Setting Machining Environment
Now we are set to get into the Manufacturing module.
 Select File →New →Manufacturing →Mill Turn
 There are many different customized CAM sessions available for different machining
operations. Here, we are only interested in the milling operation.
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9.1.3 Operation Navigator
As soon as you get into the Manufacturing environment, you will notice many changes in the main
screen such as new icons that are displayed.
 Click on the Operation Navigator tab on the right on the Resource Bar
The Operation Navigator gives information about the programs created and corresponding
information about the cutters, methods, and strategies. The list of programs can be viewed in
different categorical lists. There are four ways of viewing the list of programs in the Operation
Navigator. The four views are Program Order view, Machine Tool view, Geometry view and
Machining Method view.
 Click on Geometry View
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9.1.4 Machine Coordinate System (MCS)
 Click on the Create Geometry icon in the Insert group
to initiate setup for programming
You will see a Create Geometry pop-up. You should be able to
see the mill_contour as the program name in the Operation Navigator. If you do not see it, click
on the Geometry View button in the Toolbar again.
 Click OK
Another pop-up window will allow you to set the MCS
wherever you want. By default NX 10 takes the original
AbsoluteCS as the MCS.
 Click on the CSYS button in Specify MCS. This
will highlight the default WCS of the part and assign
it as the MCS
 Click OK to select it as the MCS
9.1.5 Geometry Definition
 Click on Geometry View
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 Expand MCS_MAIN_SPINDLE by clicking on the plus signs in the Operation
Navigator
 Double-click on WORKPIECE_MAIN in the Operation Navigator. If you do not see it,
click on other plus signs
The pop up window Workpiece Main
appears. This is where you can assign the
Part geometry, Blank geometry, and
Check geometry if any.
 Click on the Part icon
 Select the design part and click
OK
Now we have to select the Blank
Geometry.
 Click the Blank icon
This will open the Blank Geometry Window. As mentioned earlier there are several ways to assign
the Blank. You can use a solid geometry as the Blank or can allow the software to assign a prismatic
block with desired offsets in the X, Y, and Z directions. As we have already created a block we
can use that as the Blank geometry.
 Click on the Block and press OK
Now we are finished assigning the Part and Blank geometries. Sometimes it may be required to
assign Check geometry. This option is more useful for shapes that are more complex or 5-Axes
milling operations where the tool cutters have a higher chance of dashing with the fixtures. In our
case, it is not very important to assign a Check geometry.
9.2 CREATING OPERATION
9.2.1 Creating a New Operation
The manufacturing setup is now ready for us to work further with Programming Strategies. There
are many different manufacturing strategies involved in programming and it takes practice to know
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which one is the most efficient. Here, the basic guidelines are given for the most widely and
frequently used strategies. The chapter will also cover important parameters that are to be set for
the programs to function properly.
 Click on the Create Operation icon in the toolbar
The Create Operation window will pop up.
 Make sure the Type of Operation is Mill_Contour
There are many different subtypes under Mill-Contour, namely Cavity Mill, Z-Level Follow
Cavity, Follow Core, Fixed Contour, and so on. These different subtypes are used for different
situations and profiles of the design part. As mentioned before, how you select a strategy for any
situation depends on your experience.
 Click on the Cavity_Mill icon at the top left
as shown in the figure
 Change the Program from NC_PROGRAM
to 1234
 Change
the
Geometry
to
WORKPIECE_MAIN
 Click OK
The program parameters window with Cavity Mill in
the title bar will pop up. On this window, you can set
all the parameters for the program. A brief
introduction on every important parameter and
terminology will be given as we go through the
sequence.
9.2.2 Tool Creation and Selection
One of the most important decisions to make is to select the right shape and size of the tool to use.
Before starting with the Tool parameter settings, we must first know about the types of Tool
cutters. The Milling Tool Cutters are categorized into three forms of cutters. Hence, when selecting
a cutter, it is important to take into consideration the size, shape, and profiles of the design parts.
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For example, if the corner radius of a pocket is 5 mm, the pocket should be finished by a cutter
with diameter less than or equal to 10 mm. Otherwise it will leave material at the corners. There
are other special forms of cutters available in markets that are manufactured to suit this need.
Flat End Mill Cutters
These cutters have a sharp tip at the end of the cutter as shown in the figure. These cutters are used
for finishing parts that have flat vertical walls with sharp edges at the intersection of the floors and
walls.
Ball End Mill
These cutters have the corner radii exactly equal to half the diameter of the shank. This forms the
ball shaped profile at the end. These cutters are used for roughing and finishing operations of parts
or surfaces with freeform features.
Bull Nose Cutters
These cutters have small corner radii and are widely used for roughing and/or semi-finishing the
parts as well as for finishing of inclined and tapered walls.
The cutter that we are going to use to rough out this huge volume is BUEM12X1 (Bullnose End
Mill with 12 diameter and 1 corner radius).
 In the Cavity Mill pop-up menu click on the Create New button in the Tool dialog box
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 Click New
 On the New Tool window, select the Mill icon
 Type in BUEM12X1 as the Name and click
OK
This will open another window to enter the cutter
dimensions and parameters. You can also customize
the list of tools that you would normally use and call
the cutters from the library.
 Enter the values as shown in the figure below
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 Click OK
9.2.3 Tool Path Settings
Make sure that the Tool Axis is perpendicular to the top surface on the block.
 Click on Tool Axis and choose Specify Vector
 Select the appropriate axis as shown
 In the Cavity Mill menu click on the Path
Settings option
There are different options in which the tool can move.
The following is a description of each.
Follow Part: This is the most optimal strategy where
the tool path is manipulated depending on the part geometry. If there are cores and cavities in the
part, the computer intelligently considers them to remove the materials in an optimal way. This is
widely used for roughing operations.
Follow Periphery: This takes the path depending
upon the periphery profile. For example, the outer
periphery of our part is rectangular. So the tool path will
be generated such that it gradually cuts the material from
outside to inside with the Stepover value. This option is
mostly used for projections and cores rather than cavities.
Profile: This takes the cut only along the profile of
the part geometry. It is used for semi-finishing or
finishing operations.
Trochoidal: This cutter is huge and is used for removing a large amount of material. The bulk
of material is removed by gradual trochoidal movements. The depth of cut used will be very high
for this strategy.
Zig: This takes a linear path in only one direction of flow.
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Zig Zag: This tool takes a zigzag path at every level of depth. It saves time by reducing
amount of air cutting time (idle running). The climb and conventional cuts alternate.
Zig with Contour: This takes the path in one direction either climb or conventional. The
unique thing is that it moves along the contour shape nonlinearly.
 For this exercise, select the Follow Part icon from the Cut Pattern drop-down menu since
we have both projections and cavities in our part
9.2.4 Step Over and Scallop Height
Step Over
This is the distance between the consecutive passes of milling. It
can be given as a fixed value or the value in terms of cutter diameter.
The Stepover should not be greater than the effective diameter of
the cutter otherwise; it will leave extra material at every level of cut
and result in an incomplete milling operation. The numeric value or
values required to define the Stepover will vary depending on the
Stepover option selected. These options include Constant, Scallop,
Tool Diameter, etc. For example, Constant requires you to enter a
distance value in the subsequent line.
Scallop Height
Scallop Height controls the distance between parallel passes according to the maximum height of
material (scallop) you specify to be left between passes. This is affected by the cutter definition
and the curvature of the surface. Scallop allows the system to determine the Stepover distance
based on the scallop height you enter.
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 For the Stepover, select %Tool Flat and change the Percent to 70
9.2.5 Depth Per Cut
This is the value to be given between levels to slice the geometry into layers and the tool path cuts
as per the geometry at every layer. The cut depth value can vary for each level. Levels are
horizontal planes parallel to the XY plane. If we do not give cut levels, the software will
unnecessarily try to calculate slices for the entire part and machine areas that are not in our interest.
 Change the Common Depth per Cut value to be 0.5
Now we will add the level ranges. This will split the part into different levels along the Z-direction
to be machined.
 Click on Cut Levels
This will pop up a Dialog box for Cut Levels. You
need to set the level of the cut. You can either point to
the object till which the cut level is or provide it as
Range Depth value. We are not going to mill up to the
bottommost face of the part, but up to the floor at 40
mm from top. Therefore, we must delete the last level.
 Change the Range Type to User Defined
 Change the Range Depth to 80
 Select OK
9.2.6 Cutting Parameters
 On the Path Settings menu, click Cutting
Parameters
 Under the Strategy tab button, change the Cut
Order from Level First to Depth First
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Changing the cut order to Depth First orders the software to generate the tool path such that it will
mill one island completely up to the bottom-most depth before jumping to another level. The Depth
First strategy reduces the non-cutting time of the program due to unnecessary retracts and engages
at every depth of cut.
 Click on the Stock tab
 Change the value of the Part Side Stock to 0.5
This value is the allowance given to every side of the
part. If you want to give different values to the floors
(or the flat horizontal faces) uncheck the box next to
Use Floor Same As Side and enter a different value for
Part Floor Stock.
 Click OK
9.2.7 Avoidance
 Click the Non Cutting Moves
 Click the Avoidance tab
This window consists of several avoidance points of which we are concerned with the following
points:
From Point
This is the point at which the tool change command
will be carried out. The value is normally 50 or 100
mm above the Z=0 level to enhance the safety of the
job when the cutter is changed by the Automatic Tool
Changer (ATC).
 Click From Point
 Choose Specify in the Point Option field
 In the Point Dialog, enter the coordinates of
XC, YC and ZC as (0, 0, 50)
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 Choose OK
Start Point
This is the point at which the program starts and ends. This value is also 50 or 100 mm above the
Z=0 level to enhance safety. It is also the point at which the machine operator checks the height of
the tool mounted on the spindle with respect to the Z=0 level from the job. This cross checks the
tool offset entered in the machine.
 Click on Start Point
 Choose Specify
 Enter the coordinates (0, 0, 50) in the Point Dialog
 Click OK to exit the Point Constructor
Clearance Plane is the plane on which the tool cutter will retract before moving to the next region
or island. This is also known as Retract Plane. Sometimes the Clearance Plane can be the previous
cutting plane. However, when the tool has to move from one region to another, it is necessary to
move to the Clearance Plane before doing so. The value of the Clearance Plane should be at least
2 mm above the top most point of the workpiece or fixture or whichever is fixed to the machine
bed.
 Click on the Transfer/Rapid tab
 Choose Plane in the Clearance Option
 Choose the XC-YC Plane from the dropdown menu in Type tab
 Under the Offset and Reference tab enter the
value as 3 as the Distance
 Click OK twice to go back to the Cavity Mill
parameters window
9.2.8 Speeds and Feeds
 Choose Feeds and Speeds to enter the feed and speed parameters
Speed
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Speed normally specifies the rpm of the spindle (spindle speed). However, technically the speed
refers to the cutting speed of the tool (surface speed). It is the linear velocity of the cutting tip of
the cutter. The relative parameters affecting this linear speed are rpm of the spindle and the
diameter of the cutter (effective diameter).
 Enter the Spindle Speed value as 4500 rpm
For the Surface Speed and the Feed per Tooth, you should enter the recommended values given
by the manufacturers of the cutter (for this example, click on the calculator button near spindle
speed). By entering these values, the software will automatically calculate the cutting feed rate and
spindle speed. You can also enter your own values for feed rates and spindle speeds.
Feeds
There are many feeds involved in a single program.
The most important is the Cutting feed. This is the
feed at which, the tool will be in engagement with the
raw work-piece and actually cutting the material off
the work-piece. It is the relative linear velocity, at
which the cutter moves with respect to the job.
The other feeds are optional. Some machine control
systems use their default retracts and traverse feed. In
those cases, even if you do not enter the values of
other feeds, there would not be any problems. Some
control systems may look for these feed rates from the
program. It can be slightly less than the machine’s
maximum feed rate.
 Enter the Cut value as 1200 mmpm
 Click OK
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9.3 PROGRAM GENERATION AND VERIFICATION
9.3.1 Generating Program
Now we are done entering all the parameters required for the roughing program. It is time to
generate the program.
 Click on the Generate icon at the bottom of
the window
You can now observe the software slicing the model
into depths of cuts and creating tool-path at every
level. You can find on the model cyan, blue, red and
yellow lines as shown in the figure.
During the generation, you may be prompted with a
Display Parameters window.
 Uncheck the box next to Pause After Each
Path
 Then click OK to see the display of cut-levels
and tool paths
 After the generation is done, click OK in the parameters window
9.3.2 Tool Path Display
Whenever you want to view the entire tool-path of the program, right-click on the program in
Operation Navigator and click Replay. It will give the display as shown in the Figure.
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You can now observe that next to the program in the Operation Navigator is a yellow exclamation
point instead of a red mark. This means that program has been generated successfully but has not
been post-processed. If any change is made in the model, the program will again have a red mark
next to it. This implies that the program has to be generated again. However, there is no need to
change any parameters in the program.
9.3.3 Tool Path Simulation
It is very important to check the programs you have created. This prevents any improper and
dangerous motions from being made in the cutting path. It is possible that wrong parameters and
settings will be given that cause costly damages to the work piece. To avoid such mistakes, NX 10
and other CAM software provide Tool-path verification and a Gouge check.
The Tool-Path verification can be used to view the cutter motion in the entire program. You can
observe how the tool is engaged and how it retracts after cutting. It also shows the actual material
being removed through graphical simulation. You can also view the specific zone of interest by
moving the line of the program.
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 Right-click on the program in the Operation Navigator and choose Tool Path →Verify
or click on the Verify Tool Path button in the toolbar
This will allow you to set the parameters for visualization of the Tool-Path.
 On the Tool Path Visualization window, click on
the Play icon
to view the motion
You can also view the visualization in different modes by
changing the options in the drop-down menu next to
Display.
 Click on the 3D Dynamic tab on the same window
 Click on the Display Options button on the same
window
 Change the Number of Motions to 50
 Change the Animation Accuracy to Fine
 Change the IPW Color to Green
 Click OK
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 Click on the Play button
again
The simulation will look as shown in the figure on
the right. With this option, you will be able to view
the actual cutting simulation and material removal
through computer graphics. This is 3D Dynamic,
where you can rotate, pan and zoom the simulation
when it is playing. The cutting simulation is 3D.
9.3.4 Gouge Check
Gouge Check is used to verify whether the tool is removing any excess material from the workpiece
with respect to Part Geometry. Considering a Design Tolerance, any manufacturing process may
produce defective parts by two ways. One is removing excess material, which is also called Less
Material Condition. The other one is leaving materials that are supposed to be removed which is
More Material Condition. In most cases, the former is more dangerous since it is impossible to
rework the design part. The latter is safer since the leftover material can be removed by reworking
the part. The gouge check option checks for the
former case where the excess removal of material
will be identified.
 Right Click the program in the Operation
Navigator
 Choose Tool Path →Gouge Check
 Click OK
After the gouge check is completed, a message box
should pop up saying “No gouged motions found.” If
in case there are any gouges found, it is necessary to
correct the program
 Close the pop-up window which says that
there are no gauge motions found
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9.4 OPERATION METHODS
9.4.1 Roughing
In case of milling operation, the first operation should be rough milling before finishing the job.
The main purpose of roughing is to remove bulk material at a faster rate, without affecting the
accuracy and finish of the job. Stock allowances are given to provide enough material for the
finishing operation to get an accurate and good finish job. What we did in the earlier part of this
chapter is generate a roughing program. Now we have to moderately remove all the uneven
material left over from the previous program.
9.4.2 Semi-Finishing
Semi-Finishing programs are intended to remove the unevenness due to the roughing operation
and keep even part stock allowance for the Finishing operations. Once we are done with the first
roughing program, semi-finishing is always easier and simpler to perform.
Now we will copy and paste the first program in the Operation Navigator. In the new program,
you only have to change a few parameters and
cutting tool dimensions and just regenerate the
program.
 Right-click CAVITY_MILL program
in the Operation Navigator and click
Copy
 Right-click CAVITY_MILL again and
choose Paste
 Right-click the second CAVITY_MILL_COPY you just made and click Rename
 Rename the second program as CAVITY_MILL_1
You can see that next to the newly created CAVITY_MILL_1 is a red mark, which indicates that
the program is not generated.
Let us now set the parameters that need to be changed for the second program. Before we even
start, we should analyze the part geometry to figure out the minimum corner radius for the cutter
diameter. In our model, it is 5 mm and at the floor edges, it is 1 mm. Therefore, the cutter diameter
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can be anything less than 10 mm. For optimal output and rigidity, we will choose a Bull Nose
Cutter with a diameter of 10 and a lower radius of 1.
 Double-click CAVITY_MILL_1 on Operation Navigator to open the parameters
window
Just as we did in the previous program, we have to create a new cutter. In the Tool tab, you will
see the cutter you first chose. It will show BUEM12X1 as the current tool.
 Create a new Mill and name it BUEM10X1
 It should have a Diameter of 10, a Lower
Radius of 1 and a Flute Length of 38
 Click OK
 Click the Common Depth per Cut as 0.25 in
the Path Settings
 Then click on Cutting Parameters button
 Click on the Stock tab
 Uncheck the box next to Use Floor Same As
Side
 Enter 0.25 for Part Side Stock
 Enter 0.1 for Part Floor Stock
 Click on the Containment tab button
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 In the drop-down menu next to In Process Workpiece, choose Use 3D
In Process Workpiece is a very useful option in NX. The software considers the previous program
and generates the current program such that there is no unnecessary cutting motion in the Nomaterial zone. This strategy reduces the cutting time and air cutting motion drastically. The
algorithm will force the cutter to only remove that material, which was left from the previous
program and maintain the current part stock allowance.
 Choose OK to return to the Parameters window
 Click Feeds and Speeds
 Enter the Spindle Speed as 5000 and click on the Calculator
 Then click OK
The parameters and settings are finished for the semi-finishing program.
 Regenerate the program by clicking on the Generate icon
 After the software finishes generating click OK
Then replay the Tool Path Visualization. The overall Tool Path generated in the second program
will look like the following figure. You can replay it or check for the gouging in a similar way.
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9.4.3 Finishing Profile
So far, we are done with the roughing and semi-finishing programs for the part. There is a small
amount of material left in the Workpiece to be removed in the finishing programs to obtain the
accurate part geometry as intended in the design. The finishing programs should be generated such
that every surface in the part should be properly machined. Therefore, it is better to create more
than one program to uniquely machine sets of surfaces with relevant cutting parameters and
strategies rather than make one program for all the surfaces. The following illustrates how to group
the profiles and surfaces and create the finishing programs.
9.4.3.1 Outer Profile
This program is intended to finish the outer inclined walls onto the bottom of the floor. Because
the program should not touch the contour surface on the top, we have to give Check and Trim
boundaries in the program.
 Repeat the same procedure as before to copy and paste CAVITY_MILL_1 on Operation
Navigator
 Rename the program CAVITY_MILL_2
 Double click CAVITY_MILL_2 to make parameter changes
 In the pop-up parameters window, change the Cut Pattern to Profile and the Stepover
percentage to 40
 Click on the Specify Trim Boundaries tab
The Trim Boundaries window will pop up. Make sure
to carry out the following procedure in the right
sequence. Keep the default setting of Trim Side to
Inside. This tells the software that the cutter should not
cut material anywhere inside the boundary. Trim allows
you to specify boundaries that will further constrain the cut regions at each cut level.
 Change the Selection Method to Curves
 Change the Plane from Automatic to Specify and click on the Plane Dialog
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A new window will pop up. The window will ask for the mode of selection of the plane on which
the curves should be projected. This should normally be over the topmost point of the part
geometry. Precisely, it should be over the MCS.
 Choose the XC-YC Plane from the drop-down menu under Type
 Enter a value of 3 next to Distance
 Click OK
Now we will start selecting edges from the part. These selected edges will be projected on the Z =
3 plane as curves and used as the boundary.
 Select all the top outer edges on the wall along the contour surface as shown in the figure.
Make sure to select all 8 edges and in a continuous order
 Choose OK
 Enter the Common Depth per Cut as 0.2
 Click Cutting Parameters
 In the pop up dialog box, click on Stock tab
 Enter the Part Side Stock and Part Floor Stock values to be 0.00
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Intol allows you to specify the maximum distance that a
cutter can deviate from the intended path into the
workpiece.
Outtol allows you to specify the maximum distance that
a cutter can deviate from the intended path away from the
workpiece.
 Enter the Intol and Outtol values to be 0.001 as
shown in the figure
 Click on Containment tab and change the Inprocess Workpiece to None
 Click OK
 Click on the Generate icon
to generate the
program in the Main Parameters window
 Click OK on the parameters window when the program generation is completed
The finishing program for the outer profile is now ready. You can observe while replaying the tool
path that the cutter never crosses the boundary that has been given for trim and check. The cutter
retracts to the Z=3 plane for relocation.
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9.4.3.2 Inner profile
 Repeat the same procedure as before to copy and paste CAVITY_MILL_2 on Operation
Navigator and rename it as CAVITY_MILL_3
 Double-click CAVITY_MILL_3 to edit the parameters or right click on it and choose
Edit
 Select the Specify Trim Boundaries tab and choose Trim Side to be Outside in the pop
up dialog box
This will prevent the cutter from passing outside the boundary.
 Change Selection Method to Curves
 Change the plane manually to be the XC-YC plane and enter the offset distance as 3
 Click OK
 Select all the top inner edges along the contour surface as shown in the figure. Again, make
sure all 8 edges are selected in a continuous order.
 Then click OK
 Choose OK to return to the parameters window
 Generate the program
 Click OK when the generation is finished
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 Click on OK if you get any warning message about the tool fitting
The finishing program for the outer profile is now ready. By replaying the tool path, you can
observe that the cutter never crosses the boundary that has been given for trim and check.
9.4.4 Finishing Contour Surface
Now we have to use a different type of strategy to finish the top freeform surface.
 Click on the Create Operation icon
in the Toolbar
 Click on the Fixed Contour icon as shown in the figure
 Choose 1234 for Program
 Choose WORKPIECE_MAIN for Geometry
 Keep the default name of program
 Click OK
 On the Parameters window, under Drive Method, select Boundary even if it is already
shown
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If the Boundary Drive Method window still does not show up, select another Drive Method other
than Boundary, then cancel it and choose Boundary again!
 When Boundary Drive Method pups up, click on the Spanner icon as shown in the figure
to open the Boundary Geometry menu
 Change the Mode to Curves/Edges
 Select the Material Side to be Outside
 Select the Tool Position to be On
The Tool Position determines how the tool will position itself when it approaches the Boundary
Member. Boundary Members may be assigned one of three tool positions: On, Tanto, or Contact.
•
In On position, the center point of the tool aligns with the boundary along the tool axis or
projection vector.
•
In Tanto position, the side of the tool aligns with the boundary.
•
In Contact position, the tool contacts the boundary.
 For the Plane, choose User-Defined
 Again, set the plane to be XC-YC with a Distance of 3
 Click OK
 Select the outer loop of the top contour surface as shown in the figure. Remember to select
the edges in a continuous order
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 Click OK
We have trimmed the geometry outside the loop. Now we have to trim the geometry inside the
inner loop so that the only geometry left will be the area between the two loops.
 Choose the Mode to be Curves/Edges
 Choose the Material Side to be Inside and Tool Position to be On
 Choose the plane to be user-defined at XC-YC with a Distance of 3
 Select the inner edges of the contour surface as shown
 Click OK to return to the Boundary Drive Method window
 Change the Stepover method to Scallop and enter the height to be 0.001 and click OK
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 Click on Cutting Parameters
 Change the Tolerance values in the Stock tabso
that the Part Intol and Part Outtol is 0.001
 Click on the More tab button and enter the value
of Max Step as 1.0
 Click OK
 Click on the Feeds and Speeds icon on the
parameters window
 Enter the parameters as shown in the figure on
right (do not let the software calculate it)
 Click OK
In the main parameters window,
 Create a new tool and name it BEM10
 Change the diameter to be 10 mm and the lower radius to be 5 mm.
 Click OK
 Generate the program
The contour surface is now finished and you can view the
simulation by Tool Path Verification.
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9.4.5 Flooring
Flooring is the finishing operation performed on the
horizontal flat surfaces (Floors) of the part. In most of
the milling processes, flooring will be the final
operation of the process. All the horizontal surfaces
have to be finished. This planar operation runs the
cutter in a single pass on every face.
 Click on the Create Operation icon
 Change the Type to be mill_planar at the top
of the window
 Change all the options as shown in the figure
 Click OK
 In the parameters window, change the Cut
Pattern to be Follow Part
 Change the percent of the tool diameter for
Stepover to be 40
In flooring operations, it is always better to keep the
Stepover value to be less than half of the diameter of the
cutter in order to achieve more flatness on the planar
surfaces.
Unlike previous programs, we have to select a cut area.
 Click on the Specify Cut Area Floor as shown
 Select the highlighted surfaces shown in the
figure below
In case you are not able to select the surfaces as shown
go to Part Navigator and Hide the Blank, select the
surfaces and Unhide the Blank again.
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 Click OK
 Click on Cutting Parameters in the main
parameter window
 Choose the Stock tab button and enter the Intol
and Outtol values as 0.001
 Click OK
 Click on Feeds And Speeds
Because this is a Flooring operation, it is better to make
the spindle speed high and the feed rates low compared
to the previous operations.
 Enter the values exactly as shown in the figure
 Choose OK
In the main Parameters window,
 Create a new tool and name it BEF105
 Change the diameter to be 10 mm and the lower radius to be 5 mm
 Click OK
 Generate the program. Then replay and verify the cutter path
The following figure shows the Tool Path display for the flooring.
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9.5 POST PROCESSING
The primary use of the Manufacturing Application is to generate tool paths for manufacturing
parts. Generally, we cannot just send an unmodified tool path file to a machine and start cutting
because there are many different types of machines. Each type of machine has unique hardware
capabilities, requirements and control systems. For instance, the machine may have a vertical or a
horizontal spindle; it can cut while moving several axes simultaneously, etc. The controller accepts
a tool path file and directs tool motion and other machine activity (such as turning the coolant or
air on and off).
Naturally, as each type of machine has unique hardware characteristics; controllers also differ in
software characteristics. For instance, most controllers require that the instruction for turning the
coolant on be given in a particular code. Some controllers also restrict the number of M codes that
are allowed in one line of output. This information is not in the initial NX tool path. Therefore, the
tool path must be modified to suit the unique parameters of each different machine/controller
combination. The modification is called Post Processing. The result is a Post Processed tool path.
There are two steps involved in generating the final post-processed tool path.
1. Create the tool path data file, otherwise called CLSF (Cutter Location Source File).
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2. Post process the CLSF into machine CNC code (Post Processed file). This program reads
the tool path data and reformats it for use with a particular machine and its accompanying
controller.
9.5.1 Creating CLSF
After an operation is generated and saved, the resulting tool path is stored as part of the operation
within the part file. CLSF (Cutter Location Source File) provides methods to copy these internal
paths from the operations in the part file to tool paths within the CLSF, which is a text file. The
GOTO values are a "snapshot" of the current tool path. The values exported are referenced from
the MCS stored in the operation. The CLS file is the required input for some subsequent programs,
such as postprocessors.
 Click on one of the programs that
you want to post process in the
Operation Navigator
 Click on Output CLSF in the
Operations toolbar
A window will pop up to select the CLSF
Format.
 Choose CLSF_STANDARD and
enter a location for the file
 Choose OK
The CLSF file will be created. It will be similar to the figure
below. The contents of the file contain the basic algorithm of the
cutter motion without any information about machine codes and
control systems. This file can be used for post-processing any
machine control. The extension of the file is .cls (XXX.cls).
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Any program that has been output to CLSF or Post Processed will have a green checkmark next
to it in the Operation Navigator.
9.5.2 Post Processing
 Click on a program in the Operation Navigator that you want to post process
 Click Menu →Tools →Operation
Navigator →Output →Postprocess
or from the Home tab as shown below
 Select the MILL_3_AXIS machine and enter a location for the file
 Select OK
This will create the Post Processed file for the desired machine. You can find the block numbers
with G and M codes concerning the machine controller type. The extension of the file is .ptp
(XXX.ptp).
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The final output (XXX.ptp) file can be transferred to the machine and the actual milling operation
be done. This entire sequence starting from the transfer of the model into the Manufacturing
module to the transfer of the files to the machine and cutting the raw piece into the final part is
called Computer Aided Manufacturing.
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