Ansys Workbench Optimization

Prévia do material em texto

Part and Assembly Modeling
with ANSYS DesignModeler 14
Huei-Huang Lee
� � Contents� 1
Contents
Preface 2
Section A. Sketching 5
� � Exercise 1.� � Arm 6
� � Exercise 1a.� � Structural Analysis of the Arm 21
� � Exercise 2.� � Ratchet Stop 28
� � Exercise 3.� � Ratchet Wheel 35
� � Exercise 4.� � Cover Plate 44
Section B. Part Modeling 54
� � Exercise 5.� � Crank 55
� � Exercise 6.� � Geneva Gear Index 64
� � Exercise 7.� � Yoke 72
� � Exercise 8.� � Support 79
� � Exercise 8a.� � Structural Analysis of the Support 88
� � Exercise 9.� � Wheel 94
� � Exercise 10.� � Pipe 98
� � Exercise 11.� � C-Bar Dynamometer 106
� � Exercise 11a.� � Deformation of the C-Bar 111
� � Exercise 12.� � Threaded Shaft 119
� � Exercise 13.� � Lifting Fork 124
� � Exercise 14.� � Caster Frame 130
Section C. Assembly Modeling 144
� � Exercise 15.� � Threaded Shaft Assembly 145
� � Exercise 16.� � Universal Joint 152
� � Exercise 16a.� � Dynamic Simulation of the Universal Joint 165
� � Exercise 17.� � Clamping Mechanism 176
� � Exercise 17a.� � Simulation of the Clamping Mechanism 197
Section D. Concept Modeling 215
� � Exercise 18.� � 2D Solid Modeling (Arm) 216
� � Exercise 18a.� � Structural Analysis of the Arm Using 2D Model 219
� � Exercise 19.� � Surface Modeling (Support) 225
� � Exercise 19a.� � Structural Analysis of the Support Using Surface Model 230
� � Exercise 20.� � Line Modeling (Space Truss) 234
� � Exercise 20a.� � Structural Analysis of the Space Truss 240
2� Preface
Preface
Use of the Book
This book is designed for those who want to learn how to create parts and assembly models using ANSYS 
DesignModeler. The author assumes no previous CAD/CAE experiences to begin with the book.
� This book is mainly designed as an auxiliary tutorial in a course using ANSYS as a CAE platform. In particular, 
this book can serve as a preparation to the author's another book Finite Element Simulations with ANSYS Workbench 14, 
which emphasizes on finite element simulations rather than geometry modeling such that the exercises on geometry 
modeling (especially assembly modeling) may not be adequate.
ANSYS DesignModeler
ANSYS DesignModeler is a CAD program running under ANSYS Workbench environment. The DesignModeler can 
create geometries as sophisticated as any other CAD programs. Yet, many engineers choose to create geometry 
models using other CAD programs (e.g., Pro/Engineer, SolidWorks) and then import them into an ANSYS simulation 
module (such as Mechanical) for simulations. One of the reasons may be that, other than the training materials 
provided by the ANSYS Inc., there exist no tutorials in the bookstore. That is the main reason that I created this book.
� The DesignModeler is designed specifically for creating models which can be seamlessly imported into an ANSYS 
simulation modules (such as Mechanical). Therefore, if a geometry model is solely used for ANSYS simulations, I 
strongly suggest that we create the model from scratch using DesignModeler, rather than other CAD programs, to 
avoid any unnecessary incompatibilities.
Structure of the Book
There are 20 exercises and 8 appendices in the book; each of them is designed in a step-by-step tutorial style. The 20 
exercises involve creating parts and assemblies models, while the 8 appendices show how to perform simulations using 
some of the models. If you are not currently interested in simulations, you may freely skip the 8 appendices without 
affecting the learning of the 20 exercises.
� An assembly consists of two or more parts. Each part can be viewed as boolean operations (union, subtraction, 
etc.) of simpler 3D bodies. Each of the 3D bodies usually can be created by a two-step operation: drawing a 2D sketch 
on a 2D plane and then generate the 3D body by extrusion, revolution, sweeping, or skin/lofting.
� The book is divided into 4 sections. Section A lets students familiarize with sketching techniques. Section B 
contains exercises of part modeling. Section C consists of exercises of assembly modeling. The last section introduces 
the creations of concept models, including 2D models, surface models, and line models. A concept model is a 
simplification of a 3D models, and is usually easier to create and more efficient to be simulated.
� � Preface� 3
Companion Webpage
A webpage dedicated to this book is maintained by the author:
http://myweb.ncku.edu.tw/~hhlee/Myweb_at_NCKU/ADM14.html
The webpage contains links to finished project files of each exercise and appendix. If everything works smoothly, you 
do not need them at all. Every model can be built from scratch according to the steps described in the book. The 
author provides these project files just in some cases you need them. For examples, if you have troubles to follow the 
geometry details in the textbook, you may need to look up the geometry details from the project files.
Huei-Huang Lee
Associate Professor
Department of Engineering Science
National Cheng Kung University
Tainan, Taiwan
hhlee@mail.ncku.edu.tw
myweb.ncku.edu.tw/~hhlee
4�
� � Section A. Sketching� 5
Section A
Sketching
An assembly is a combination of parts. From manufacture point of view, a part is a basic unit for manufacturing 
process. Many parts can be created by a two-step operation: drawing a 2D sketch on a plane and then generate a 3D 
body by extrusion, revolution, sweeping, or skin/lofting.
� The exercises in Section A are designed to introduce the 2D sketching techniques provided by the 
DesignModeler. Each part created in Section A involves drawing a sketch and then extrude to generate a 3D solid 
body representing the part.
� Although it can be used as a general purpose CAD software, the DesignModeler is particularly designed for 
creating geometric models to be analyzed (simulated) under the ANSYS environment. To let the readers understand 
what it means by analysis (simulation) as early as possible, an exercise (Exercise 1a) is appended right after Exercise 1 
to perform a structural analysis for the part created in Exercise 1. However, the reader has option to skip Exercise 1a 
without affect the subsequent learning of geometric modeling.
6� Exercise 1. Arm� �
 X
 Y
 1.375
 2
.2
5
 
Unit: in.
Thickness: 0.125 in.
 R0.5
 3×D0.25
 R0.313
 R0.25
 R0.313
[2] Details of 
the arm.
[3] The global 
coordinate 
system.
[1] The arm is a part 
of a clamping 
mechanism. 
Exercise 1
Arm
In this exercise, we will create a 3D 
solid model for an arm, which is a 
part of a clamping mechanism [1]. 
The clamping mechanism will be 
introduced in Exercise 17 and 
simulated in Exercise 17a.
� The arm model consists of a 
single solid body, which can be 
generated by extruding a sketch by a 
thickness of 0.125 inches [2].
� Before creating a geometry 
model, we must set up a global 
coordinate system. For this exercise, 
we arbitrarily choose the global 
coordinate system as shown [3]. 
Note that the origin is on the back 
surface of the part.
1-1 Introduction
� � Exercise 1. Arm� 7
[2] The <Workbench GUI> 
(graphical user interface) shows up.
[3] Click the plus sign (+) to 
expand <Component 
Systems>. The plus sign 
becomes minus sign.
[4] Double-click to create 
a <Geometry> system.
[7] Double-click 
<Geometry> to start 
up the DesignModeler.
[6] You may click here to 
show the messages from 
ANSYS Inc. To hide the 
message, click it again.
[1] Launch ANSYS 
Workbench.
1-2 Start Up DesignModeler
[5] A <Geometry> system 
is created in the <Project 
Schematic> area.
8� Exercise 1. Arm� �[10] Click <OK>. Note 
that, after clicking and 
entering DesignModeler, the 
length unit cannot be 
changed anymore.
[9] Select <Inch> as 
length unit.
[8] <DesignModeler GUI> 
shows up.
Speech Bubbles
1. In this book, each exercise is divided into subsections (e.g., 1-1, 1-2). In each subsection, speech bubbles are 
ordered with numbers, which are enclosed by pairs of square brackets (e.g., [1], [2]). When you read, please follow 
the order of speech bubble; the order is significant.
2. The square-bracket numbers also serve as reference numbers when referred in other text. When in the same 
subsection, we simply refer to a speech bubble by its number (e.g., [1], [2]). When in the other subsections, we refer 
to a speech bubble by its subsection identifier and its bubble number (e.g., 1-2[1]).
3. When a circle is used with a speech bubble, it is to indicate that mouse or keyboard ACTIONS are needed in that 
step [1, 3, 4, 7, 9, 10]. A circle may be filled with white color [1, 4, 7] or unfilled [3, 9, 10]. A speech bubble without a 
circle [2, 8] or with a rectangle [6] is used for commentary only, i.e., no mouse or keyboard actions are needed.
Workbench Keywords
A pair of angle brackets is used to highlight an Workbench keyword (e.g., <Component Systems> in [3]). 
Sometimes, if the angle brackets do not add any clarity, they may be dropped (e.g., DesignModeler).
Clicking and Selecting
When we say "click" or "select," we mean left-click the mouse button.
� � Exercise 1. Arm� 9
1-3 Prepare to Draw a Sketch on <XYPlane>
[1] By default, 
<XYPlane> is the 
current sketching 
plane (active plane).
[2] Click to switch to <Sketching 
Mode>. Note that there are 5 
toolboxes available: Draw, Modify, 
Dimension, Constraints, and Settings. 
<Draw> is the default toolbox.
[3] Click <Look 
At Face/Plane/
Sketch> to rotate 
the view angle so 
that you look at the 
current sketching 
plane.
[4] By default, the ruler is 
on. In the next step, we will 
turn off the ruler to make 
more sketching space.
[5] Select <View/
Ruler> to turn it off. 
For the rest of this 
book, we always leave 
the ruler off.
[6] This is the global 
coordinate system.
[7] This is the plane 
(local) coordinate 
system.
10� Exercise 1. Arm� �
1-4 Draw a Circle with Dimension
[1] Select 
<Circle> tool.
[2] In case you don't 
see the <Circle> tool, 
scroll down to reveal 
the tool.
[3] It gives you hints for 
using the tool.
[4] Move the mouse 
around the origin until 
a <P> (Point) appears 
and then click the 
mouse to locate the 
center of the circle. 
The ability to "snap" a 
point is a feature of the 
DesignModeler, called 
<Auto Constraints>.
[5] Move the mouse 
away from the center and 
then click the mouse to 
create a circle with 
arbitrary radius.
[7] Select 
<Dimension> 
toolbox.
[8] Select 
<Diameter> tool.
[9] Select the circle, 
move the mouse 
outward, and then click 
to create a dimension. 
Note that the circle turns 
blue, meaning the circle 
has fully constrained 
(fixed in the space).
[10] In the <Details 
View>, type 0.25 for 
the diameter.
[11] It is possible that the circle 
becomes too small. Select <Zoom to 
Fit> tool to fit the sketch into the 
graphics window. Now, we may need 
to adjust (move) the position of the 
dimension. 
[6] As soon as you 
begin to draw, a name 
is assigned to the 
sketch and it becomes 
the active sketch.
� � Exercise 1. Arm� 11
[12] Select <Move> tool. 
Remember to scroll 
down to reveal a tool if 
you don't see the tool.
[13] Select the 
dimension, move to a 
suitable position, and 
then click again.
[14] Whenever necessary, select 
<Zoom to Fit> tool to fit the 
sketch into the graphics window. 
[15] Select <Display> 
tool. You may need to 
scroll down to reveal 
the tool if you don't see 
the tool.
[16] Click <Name> to 
turn the dimension 
name off. Note that 
<Value> automatically 
turns on.
[17] Instead of displaying dimension 
name, now the dimension value is 
displayed. For the rest of the book, 
we always display dimension values 
instead of name.
12� Exercise 1. Arm� �
1-5 Draw Two More Circles
[1] Click anywhere in the 
graphics window and then scroll 
the mouse wheel down to zoom 
out the sketch roughly like this.
[2] Select <Draw> 
toolbox.
[4] Move the mouse 
around the horizontal 
axis until a <C> 
(Coincident) appears 
and then click the 
mouse to locate the 
center of the circle. 
This center is snapped 
on the horizontal axis.
[5] Move the mouse until an <R> 
(Radius) appears and then click the 
mouse. The radius dimension is 
constrained to be the same as the 
first circle. Note that the circle is 
greenish-blue, meaning it is not 
fully fixed in the space yet. A 
horizontal location is needed to 
fully defined the circle.
[6] Create another circle in a 
similar way. Make sure a <C> and 
an <R> appear before clicking. A 
vertical location is needed to fully 
defined the circle.
[3] Select 
<Circle> tool.
� � Exercise 1. Arm� 13
[7] Select 
<Dimension> toolbox 
and then select 
<Horizontal> tool.
[8] Select the vertical 
axis. Note that the shape 
of the mouse cursor 
changes when your mouse 
is on the axis.
[9] Select the center of 
the circle. Note that the 
shape of the mouse 
cursor changes when your 
mouse is on the point.
[10] Move the mouse upward roughly 
here and click to locate a horizontal 
dimension. Note that the circle turns 
blue (fully constrained).
[11] In the <Details 
View>, type 1.375 for 
the horizontal 
dimension.
[12] Remember that you 
always can use <Zoom to Fit> 
and scroll the mouse wheel [1] 
to zoom in/out the view. Also, 
to "pan" the view, simply move 
the mouse while holding the 
control-middle-button.
[13] Select 
<Vertical> tool.
[14] Select horizontal axis, 
select the center of the lower 
circle, move the mouse 
leftward roughly here, and click 
to locate a vertical dimension. 
The circle turns blue.
[15] In the <Details 
View>, type 2.25 for 
the vertical 
dimension.
[16] Before going further, make sure you 
familiarize the two most frequently used view 
operations: scrolling the mouse wheel to zoom 
in/out the view and moving mouse with 
control-middle-button to pan the view.
14� Exercise 1. Arm� �
1-6 Draw Three Concentric Circles
[1] Select the <Draw/
Circle> tool, and draw a 
concentric circle. Make sure 
a <P> appears before 
defining the center.
[2] Select the <Dimension/
Radius> tool, and create a 
radius dimension for the 
circle. In the <Details 
View>, type 0.313 for the 
radius.
[3] Select the <Draw/Circle> tool, 
and draw a concentric circle with the 
same radius as the previous circle. 
Make sure a <P> appears before 
defining the center and an <R> 
appears before defining the radius.
[4] With the <Draw/Circle> 
tool still selected, draw a 
concentric circle. Make sure a 
<P> appears before defining 
the center. 
[5] Select the <Dimension/
Radius> tool, and create a 
radius dimension for the 
circle. In the <Details 
View>, type 0.5 for the 
radius.
� � Exercise 1. Arm� 15
1-7 Draw Tangent Lines
[1] Select the <Draw/Line 
by 2 Tangents> tool, and 
then select the two circles 
to be tangent to. A tangent 
line is created.
[2] Create additional 
three tangent lines in a 
similar way.
16� Exercise 1. Arm� �
1-8 Draw a Fillet
[1] Select the <Modify/
Fillet> tool, and type 0.25 
for <Radius>.
[2] Select these two lines. 
A fillet is created. Note 
that the fillet is not blue-
colored. We need to 
specify the radius. The 
radiustyped in [1] is not 
necessarily the final 
dimension; it just serves as 
a default dimension.
[3] Select the <Dimension/Radius> 
tool, and create a radius dimension for 
the fillet. You don't need to type in the 
<Details View>, since the default value 
[1] is automatically used. Note that the 
color turns blue now.
� � Exercise 1. Arm� 17
1-9 Trim Away Unwanted Segments
[1] Select the <Modify/
Trim> tool, and turn on 
<Ignore Axis>, meaning 
that the axes will not serve 
as trimming tools.
[2] Click the circle 
roughly here to trim 
away the arc. Note 
that when you select 
an edge (a line or a 
curve), the remaining 
edges will serve as 
trimming tools.
[3] Click to trim 
away two other 
arcs.
[4] The sketch after 
trimming.
18� Exercise 1. Arm� �
1-10 Extrude the Sketch to Create the Arm
[1] Select 
<Extrude> tool.
[2] It automatically 
switches to 
<Modeling Mode>, in 
which a <Tree 
Outline> is 
displayed, which will 
be explained later.
[3] Click the 
little cyan sphere 
to rotate the 
view into an 
isometric view.
[4] Type 0.125 for 
the <Depth>.
[6] Click <Generate> 
to produce a 3D solid 
body.
[7] Click <Display 
Plane> to turn off the 
display of XYPlane (and 
the sketches it contains).
1-11 Save the Project and Exit Workbench
[1] Select <File/Close 
DesignModeler>. The 
<DesignModeler GUI> 
disappears.
[2] In the <Workbench 
GUI>, save the project 
as "Arm." 
[3] Select <File/
Exit> to quit 
from the 
Workbench.
[5] The active sketch is 
automatically taken as 
<Geometry>.
� � Exercise 1. Arm� 19
Global Coordinate System
Before creating a geometry model, you must set up a global coordinate system (1-1[3], 1-3[6]).
Workbench GUI
In the <Workbench GUI> (1-2[2]), you can create a system (1-2[4]) and start up DesignModeler (1-2[7]). Other 
capabilities will be introduced later.
Project Schematic
Created systems appear on the <Project Schematic>, an area in the <Workbench GUI>.
DesignModeler GUI
Geometries are created entirely within the <DesignModeler GUI> (1-2[8]).
Length Unit
Before creating a model in the DesignModeler, you must choose a length unit (1-2[9, 10]). The length unit cannot be 
changed thereafter.
Mouse Operations
Click�� � -- � Left-click the mouse button.
Select� � -- � Left-click the mouse button.
Double-Click� -- � Left-click the mouse button twice.
Zoom In/Out� -- � Scroll the mouse wheel
Pan� � � -- � Move the mouse while holding control-left-button.
Other mouse operations will be introduced later.
Current Sketching Plane
Each sketch is stored in the current sketching plane (1-3[1]). Manipulating (switching, creating, etc.) sketching planes 
will be introduced later.
Sketching Mode v.s. Modeling Mode
Tools for sketching are provided in the <Sketching> mode (1-3[2]), while tools for creating and manipulating bodies 
are provided in the <Modeling> mode (1-10[2]). There are 5 toolboxes available: Draw, Modify, Dimension, 
Constraints, and Settings. Tools in <Modeling> mode includes <Extrude> (1-10[1]). Some tools are available in both 
modes, e.g., <Zoom To Fit> (1-4[11]).
Look At Face/Plane/Sketch
Clicking this tool to rotate the view angle so that you look at the current sketching plane (1-3[3]).
Ruler
The ruler (1-3[4, 5]) is to help you obtain a better feeling of the drawing scale. In this book, we always leave the ruler 
off to make more sketching space.
Plane Coordinate System
Every plane has its own coordinate system (1-3[7]); it is also called a local coordinate system. The plane coordinate 
system will be explained further later.
1-12 Review
20� Exercise 1. Arm� �
Scrolling
In case you don't see a tool in a toolbox, scroll down/up to reveal the tool (1-4[2]). There is also a scrolling controller 
for the <Details View>.
Tools in <Draw> Toolbox
Circle� � � -- Draw a circle, giving the center and the radius (1-4[1, 3-5]).
Line by 2 Tangent� -- Draw a line tangent to two curves (including circles and arcs) (1-7[1, 2]).
Tools in <Dimension> Toolbox
Radius� � -- � Specify a radius dimension by selecting a circle (1-4[6, 8-10]) or an arc (1-8[2]).
Move�� � -- � Move (relocate) a dimension name/value by dragging the name/value (1-4[12, 13]).
Display� � -- � This tool is to toggle the display of dimension name and the dimension value (1-4[15-17]).
� � � � In this book, we always turn off the dimension name and turn on the dimension value.
Horizontal�� -- � Specify a horizontal dimension by first selecting a or a point (or a vertical line) and
� � � � then a second point (or a vertical line) (1-5[7-10]).
Vertical� � -- � Specify a vertical dimension by first selecting a or a point (or a horizontal line) and
� � � � then a second point (or a horizontal line) (1-5[13, 14]).
Tools in <Modify> Toolbox
Fillet� � -- � Create a fillet by selecting two lines or curves (1-8[1-3]).
Trim� � -- � Trim away unwanted segments (1-9[1-4]).
Auto Constraints
P� -- � The mouse cursor snaps to a point (or the origin) (1-4[4]).
R� -- � The radius is the same as another circle (or arc) (1-4[5]).
C� -- � The mouse cursor is coincident to a line (or an axis) (1-5[4, 6]).
Other auto constraint features will be introduced later.
Color Codes
Greenish-blue� -- � Under-constrained (1-8[2])
Blue� � � -- � Fully constrained (fixed in the space) (1-4[9], 1-5[10,14]).
Red� � � -- � Over-constrained
Zoom To Fit
Click this tool to fit the entire sketch (in the <Sketching> mode) or entire model (in the <Modeling> mode) into the 
graphics window (1-4[14]).
Extrude
This tool extrude a sketch by a specified depth to create a 3D body (1-10[1-5]). More exercises will be given later.
Isometric View
Click the little cyan sphere of the triad will rotate the view into an isometric view (1-10[3]). Other view controls will 
be introduced later.
Display Plane
This tool is to toggle the display of current sketching plane and the sketches it contains (1-10[6]).
� � Exercise 1a. Structural Analysis of the Arm� 21
[2] This is the deformed 
structure under the design 
loads. The wireframe is the 
underformed configuration. 
Note that, for visual effects, 
the deformation has been 
exaggerated. 
Appendix:
Exercise 1a
Structural Analysis of the Arm
Although it can be used as a general purpose 
CAD software, the DesignModeler is 
particularly designed for creating geometric 
models to be analyzed (simulated) under the 
ANSYS environment. The purpose of this 
exercise is to let the readers understand what 
it means by analysis (simulation). However, the 
reader has option to skip this exercise without 
affect the subsequent learning of geometric 
modeling.
� In this exercise, we will perform a static 
structural analysis for the arm created in 
Exercise 1. The objective is to find the 
deformation and stresses under the working 
loads.
� The clamping mechanism is entirely 
made of steel and is designed to withstand a 
clamping force of 450 lbf [1]. After a 
structural analysis of the entire mechanism [2] 
(also see Exercise 17a), the results show 
shows that, to withstand a clamping force of 
450 lbf, the arm is subject to external forces as 
shown [3] (also see 17a-13). Note that the 
external forces are in a state of static 
equilibrium.
� The analysis for the entire clamping 
mechanism will be perform in Exercise 17a. In 
this exercise, we will only perform a analysis 
on the arm. The purpose is to make sure the 
stresses are within the allowable stress of the 
steel, which is 30,000 psi.
� The analysis task cannot not be 
performed in DesignModeler. Rather, it is 
carried out with <Mechanical>, another 
Workbench application program.
1a-1 Introduction
[1] The clamping 
mechanism is 
designed to withstand 
a clamping force of 
450 lbf.281 lbf
 126 lbf
 264 lbf 187 lbf
 407 lbf
 77 lbf
[3] The external 
forces on the arm. 
These forces are 
calculated 
according to 
17a-13.
22� Exercise 1a. Structural Analysis of the Arm
[2] Open the project "Arm," 
which was saved in Exercise 1.
[1] Launch ANSYS 
Workbench.
1a-2 Start Up <Mechanical>
[3] Double-click to create 
a <Static Structural> 
analysis system.
[4] Drag <Geometry>...
[5] And drop here. A link 
is created, indicating that 
both <Geometry> share 
the same data.
[6] Double-click to 
start up the 
<Mechanical>.
� � Exercise 1a. Structural Analysis of the Arm� 23
[7] This is the <Mechanical> GUI. Note 
that the model is automatically brought 
into <Mechanical>. By default, the body 
is assumed to be made of steel.
[8] Make sure the length 
unit is <in.>. If not, 
select the right unit from 
the pull-down menu 
<Units> (see [9]).
[9] If the length unit is not <in.>, 
select <Units/U.S. Customary (in, 
lbm, lbf, F, s, V, A)>. Unlike 
DesignModeler, the units can be 
changed any time as you like in 
<Mechanical>.
24� Exercise 1a. Structural Analysis of the Arm
1a-3 Specify Loads
[1] Click to highlight 
<Static Structural>.
[2] Select <Loads/
Force>.
[3] A <Force> object is 
inserted under the <Static 
Structural> branch.
[4] Select this 
cylindrical face.
[5] Click <Apply>.
[6] Select <Components>.
[7] Type -187 (lbf) for <X 
Component>, and 126 (lbf) 
for <Y Component>.
[8] Select <Loads/
Force> again.
[9] A <Force 2> object 
is inserted.
[10] Select this 
cylindrical face.
[11] Click 
<Apply>.
[12] Select <Components>.
[13] Type 264 (lbf) for <X 
Component>, and 281 (lbf) 
for <Y Component>.
� � Exercise 1a. Structural Analysis of the Arm� 25
[1] Select <Supports/
Fixed Support>.
[2] A <Fixed Support> is 
inserted.
[4] Click 
<Apply>.
[3] Select this 
cylindrical face.
1a-4 Specify Supports
1a-5 Insert Result Objects
[1] Click to highlight 
<Solution>.
[3] A solution object is 
inserted under the 
<Solution> branch.
[2] Select <Stress/
Equivalent (von-Mises)>.
26� Exercise 1a. Structural Analysis of the Arm
1a-6 Solve the Model
[1] Click <Solve>.
[7] Click to close the 
<Message> window.
[8] Click <Play> to 
animate the 
deformation.
[9] Click <Stop> to 
stop the animation.
[2] Click the Z-axis 
to rotate the view so 
that you look into the 
<XYPlane>.
[3] The maximum stress 
is 29,690 psi, slightly below 
the allowable stress 
(30,000 psi). Note that the 
maximum stress can be 
reduced by increasing the 
radius of the fillet.
[6] For visual 
effect, the 
deformation is 
automatically 
enlarged 49 times. [5] Undeformed 
shape.
[4] Select <Edges/
Show Undeformed 
WireFrame>.
� � Exercise 1a. Structural Analysis of the Arm� 27
1a-7 Save the Project and Exit Workbench
[1] Select <File/Close 
Mechanical>. The 
<Mechanical GUI> 
disappears.
[2] In the <Workbench 
GUI>, save the project as 
"Arm-a". 
[3] Select <File/
Exit> to quit from 
the Workbench.
28� Exercise 2. Ratchet Stop� �
Exercise 2
Ratchet Stop
The ratchet stop is used to control a 
ratchet wheel so that the ratchet 
wheel rotates in a certain direction 
only [1, 2]. The ratchet wheel will be 
created in Exercise 3. In this exercise, 
we'll create a 3D solid model for the 
ratchet stop.
� The details of the ratchet stop 
are shown in the figure below [3]. 
Note that the coordinate system is 
also shown in the figure.
2-1 Introduction [2] The ratchet stop is used to control the 
rotational direction of 
the ratchet wheel.
[1] The ratchet 
wheel.
 Y
 X
 0.57
 0
.1
25
 
Unit: in.
Thickness: 0.125 in.
 R0.56
 R0.188
 R0.34
 0
.16 
Slo
p: 
40
�
[3] Details 
of the 
ratchet stop.
� � Exercise 2. Ratchet Stop� 29
[2] Double-click 
<Geometry> cell to start 
up the DesignModeler. 
Select <Inch> as the length 
unit (1-2[9, 10]).
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system 
(1-2[1-5]).
2-2 Start Up DesignModeler
2-3 Draw a Circle on XYPlane
[1] Switch to 
<Sketching 
Mode> (1-3[2]).
[2] Rotate to 
XYPlane view 
(1-3[3])
[3] Draw a 
circle centered at 
the plane origin 
(1-4[1-5]).
[4] Select <Dimension/Radius> tool and 
specify a radius of 0.188 (in.) for the circle. 
Remember to turn on the display of dimension 
value (1-4[15-17]). Also remember to use 
<Dimension/Move> to move the dimension to 
a suitable position (1-4[12, 13]).
30� Exercise 2. Ratchet Stop� �
2-4 Draw a Line
[1] Select <Draw/
Line> tool and 
draw a line 
roughly like this.
[2] Select <Dimension/General> 
tool and create a length 
dimension by simply selecting 
the line segment and move the 
mouse upward. Specify a 
dimension value of 0.16 (in.).
[3] Select <Dimension/Horizontal> 
tool and specify a horizontal 
dimension of 0.57 (in.) (1-5[7-11]).
[4] Select <Dimension/
Vertical> tool and specify 
a vertical dimension of 
0.125 (in.) (1-5[13-15]).
[5] The line is not blue-
colored, meaning it isn't fully 
defined in the space yet. We 
now specify an angle dimension 
for the line.
2-5 Specify an Angle Dimension
[1] To specify an angle dimension, you need to select two lines (or axes). 
When you select a line (or axis), the end near where you click become 
the "arrow end" of the line. The angle is then measured from the first 
line to the second line in a counter-clockwise fashion. 
[2] Select <Dimension/
Angle> tool and then 
click the X-axis on the 
positive side.[3] Click the line 
here near the 
upper-right end.
[4] Click here to create 
an angle dimension. 
Type 40 (degrees) in the 
<Details View>. Note 
that the angle is 
measured counter-
clockwise from the first 
line to the second. Also 
note that the line is 
blue-colored now.
[5] If you made mistakes (click on wrong ends or in a wrong order) and the 
angle is not what you meant, right-click anywhere in the graphics window to 
bring up a <Context Menu> and choose <Alternate Angle>. Repeat this before 
you click to locate the angle dimension until the correct angle appears.
� � Exercise 2. Ratchet Stop� 31
2-6 Draw Arcs
[1] Select <Draw/Arc by 
Center> tool and then 
click roughly here to 
define the center.
[3] Click to define 
another end roughly 
here on the circle.
[2] Click the upper-
right end of the line 
to define an end of 
the arc.
[4] An arc is created.
[5] Select <Dimension/
Radius> tool and 
specify a radius 
dimension of 0.56 in. [6] Select <Constraints/
Tangent> tool and then select 
the arc and the circle. A 
<Tangent> constraint is 
imposed between the arc and 
the circle. Note that the arc 
turns blue.
[7] Also note that the center of the 
arc moves to a new location to 
accommodate the constraint.
32� Exercise 2. Ratchet Stop� �
[8] Select <Draw/Arc by 
Center> tool again and 
define the center roughly 
here.
[9] Click the lower-
left end of the line to 
define an end of the 
arc.
[10] Click to define 
another end roughly 
here on the circle.
[11] Select <Dimension/
Radius> tool and specify 
a radius dimension of 
0.34 in.
[12] Select <Constraints/
Tangent> tool and impose a 
<Tangent> constraint 
between the newly created 
arc and the circle.
� � Exercise 2. Ratchet Stop� 33
2-7 Trim Away Unwanted Segments
[1] Select <Modify/Trim> tool 
and make sure <Ignore Axis> is 
turned on (1-9[1]). Click here 
to trim away the arc segment.
[2] The finished sketch.
2-8 Extrude the Sketch to Create the Ratchet Stop
[1] Extrude the sketch 
0.125in. to create the 
ratchet stop (1-10[1-6]).
Wrap Up
Close DesignModeler, save the project as "Stop," and exit the 
Workbench (1-11[1-3]).
34� Exercise 2. Ratchet Stop� �
Context Menu
When you right-click the mouse, a menu pops up. The contents of the menu 
depends on when and where you right-click the mouse. The menu is thus 
called the <Context Menu> (2-5[5]). Try to right-click anywhere in the 
graphics area, <Details View>, or <Tree Outline> (1-10[2]), to see the 
contents of the <Context Menu>.
<Dimension/General> Tool
This tool can be used for any type of dimension. For a line, the default is to 
create a <Length> dimension (2-4[2]). For a circle or arc, the default is to 
create a diameter dimension. If the default is not what you want, right-click 
anywhere in the graphics window to bring up the <Context Menu> [1] and 
choose a dimension type.
<Dimension/Angle> Tool
To specify an angle dimension, you need to select two lines (or axes). When 
you select a line (or axis), the end near where you click become the "arrow 
end" of the line. The angle is then measured from the first line to the second 
line in a counter-clockwise fashion (2-5[1-4]).
� If you made mistakes (click on wrong ends or in a wrong order) and 
the angle is not what you meant, right-click anywhere in the graphics window 
to bring up the <Context Menu> [2] and choose <Alternate Angle>. Repeat 
this until the correct angle appears before you click to locate the angle 
dimension (2-5[5]).
<Draw/Line> Tool
This tool draws a line by defining two end points (2-4[1])).
<Draw/Arc By Center> Tool
This tool draws an arc by defining its center and two end points (2-6[1-4]).
<Constraints/Tangent> Tool
This tool impose a <Tangent> constraint between two curves or between a 
line and a curve (2-6[6, 12]). 
2-9 Review
[1] This is the 
<Context Menu> when 
<Dimension/General> is 
activated.
[1] This is the <Context 
Menu> after you select 
two lines (or axes) and 
before you click to create 
an angle dimension.
� � Exercise 3. Ratchet� 35
Exercise 3
Ratchet Wheel
In this exercise, we'll create a 3D 
solid model for the ratchet wheel 
mentioned in Exercise 2 [1]. The 
details of the ratchet wheel are 
shown in the figure below [2].
3-1 Introduction
[1] The ratchet 
wheel.
 Y
 X
 
Unit: in.
Thickness: 0.25 in.
 D0.25
 1.
00
 15�
 60 �
[2] Details of 
the ratchet 
wheel.
36� Exercise 3. Ratchet
[2] Double-click 
<Geometry> cell to start 
up the DesignModeler. 
Select <Inch> as the length 
unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
3-2 Start Up DesignModeler
3-3 Draw Two Concentric Circles
[1] On XYPlane, draw two 
concentric circles with 
diameters of 0.25 in. and 
1.00 in. respectively.
� � Exercise 3. Ratchet� 37
3-4 Draw Lines with Angle Dimensions
[1] Draw a line passing 
the origin like this.
[2] Specify an angle dimension 
of 15 degrees. Remember to 
select the line first and then 
the axis. Clicking positions are 
also important (2-5[1-5]).
[3] Draw 
another line like 
this.
[4] Specify an angle 
dimension of 60 
degrees.
38� Exercise 3. Ratchet
3-5 Trim Away Unwanted Segments
[1] Draw a circle which passes 
through an end point of the line. 
When you define the radius, 
remember to snap (with a <P> 
constraint) the end point of the line. 
The circle serves as a construction 
(temporary) circle.
[2] Trim away 
unwanted segments. 
Remember to turn on 
<Ignore Axis> (1-9[1]).
[3] After 
trimming, a single 
tooth remains.
� � Exercise 3. Ratchet� 39
3-6 Duplicate Teeth
[1] Select 
<Modify/Copy>.
[2] Select these two lines. To 
select multiple entities, hold 
Control key while click the 
entities sequentially. You also can 
"sweep select" multiple entities, 
i.e., holding left mouse button 
while sweep through the entities. 
After the selection, the entities 
are highlighted with yellow color.
[3] Right-click 
anywhere in the 
graphics window to 
bring up the 
<Context Menu>, and 
select <End/Use Plane 
Origin as Handle>. 
Now the tooth has 
been copied to a 
"clipboard."
[4] The <Modify/Paste> 
tool is automatically 
activated. Type 15 
(degrees) for the <r>, 
meaning that the rotating 
angle is 15 degrees.
40� Exercise 3. Ratchet
[5] Bring up the 
<Context Menu>, 
and select <Rotate by 
-r Degrees>. Note 
that a negative angle 
is to rotate 
clockwise. [6] Bring up the 
<Context Menu> 
again, and select 
<Paste at Plane 
Origin>.
[7] The tooth is 
rotated 15 degree 
clockwise (using 
plane origin as 
center of 
rotation) and 
pasted.
[8] Repeat steps [5, 6] 
four more times. Press 
<Esc> to end the tool 
or choose <End> from 
the <Context Menu>.
� � Exercise 3. Ratchet� 41
[9] Select <Modify/
Copy> again, and 
select all the teeth, 
using "sweep 
select" [2]. From the 
<Context Menu>, 
select <End/Use 
Plane Origin as 
Handle> [3].
[10] Type 90 
(degrees) for the 
rotating angle.
[11] Repeat 
steps [5, 6].
[12] Repeat steps [5, 6] two 
more times. Press <Esc> to 
end the tool or choose <End> 
from the <Context Menu>.
42� Exercise 3. Ratchet
3-7 Extrude the Sketch to Create the Ratchet Wheel
Wrap Up
Close DesignModeler, save the project as "Ratchet," and exit 
the Workbench.
[1] Extrude the sketch 0.25 
in. to create the ratchet 
wheel.
� � Exercise 3. Ratchet� 43
Selection of Multiple Entities
There are several ways to select multiple entities. Two of them are <Control-Select> and <Sweep Select>.
� Control-Select� --� Click the entities sequentially while holding the Control key.
� Sweep Select� --� Hold the left mouse button and sweep through the entities.
� Box Select�� --� Select <Select Mode/Box Select> [1], and use mouse to define a box.
� � � � � All entities inside the box are selected.
3-8 Review
<Modify/Copy> and <Modify/Paste> Tools
<Modify/Copy> copies the selected entities to a "clipboard." A <Paste Handle> must be specified using one of the 
methods in the <Context Menu> (3-6[3]). After completing the <Copy> tool, the <Paste> tool is automatically 
activated.
� <Modify/Paste> pastes the entities in the "clipboard" to the graphics window. The pasting location corresponds 
to the <Paste Handle> specified in the <Copy> tool. To define the pasting location, you either click on the graphics 
window or choose from the <Context Menu> (3-6[6]). Many options also can be chosen from the <Context Menu> 
(3-6[5]), where the rotating angle <r> and the scaling factor <f> can be specified with the tool (3-6[4]). A positive 
rotating angle is to rotate counter-clockwise.
<Modify/Replicate> Tool
<Replicate> is equivalent to a <Copy> followed by a <Paste>.
Ending a Tool
You can press <Esc> to end a tool (3-6[8, 12]). Besides, the <Context Menu> often provides an <End> option to end 
a tool (3-6[5, 6]).
[1] One way to select 
multiple entities is to 
turn on <Select Model/
Box Select>.
44� Exercise 4. Cover Plate� �
Exercise 4
Cover Plate
In this exercise, we'll create a 3D solid model 
for a cover plate, of which the details are 
shown in the figure below [2].
4-1 Introduction
 Y
 X
 
Unit: in.
Thickness: 0.046 in.
 8 ×R0.15
 2
.0
0
[1] Details of 
the cover plate.
 0.376
 1.
25
 0
.7
5
 0
.2
5
 0
.2
5
 0.562
 1.50
 6 ×R0.06
 0.312 0.312
 2 ×R0.188 2 ×D0.201
� � Exercise 4. Cover Plate� 45
[2] Double-click 
<Geometry> cell to start 
up the DesignModeler. 
Select <Inch> as the length 
unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
4-2 Start Up DesignModeler
4-3Draw Circles
[1] On XYPlane, draw a 
circle centered at the 
origin and with a diameter 
of 0.201 in.
[2] Draw another circle 
with the same diameter. 
Make sure an <R> appears 
when you define the radius 
(1-5[5]).
[3] Use <Dimension/
Horizontal> to specify a 
dimension of 0.376 in.
[4] Use <Dimension/
Vertical> to specify a 
dimension of 2 in.
46� Exercise 4. Cover Plate� �
[5] Draw a concentric 
circle with a radius of 
0.188 in.
[6] Draw a concentric 
circle with the same radius. 
Make sure an <R> appears 
when you define the radius.
4-4 Draw Rectangles and Lines
[1] Select <Draw/
Rectangle> and draw a 
rectangle with 
dimensions a shown.
� � Exercise 4. Cover Plate� 47
[2] Select <Draw/Polyline> and 
draw three segments like this. 
Select <Open End> from the 
<Context Menu> after you 
define the fourth point. Note 
that the three segments are 
either horizontal or vertical, 
therefore make sure an <H> or 
a <V> appears before clicking. 
Specify the dimensions as 
shown.
[3] Select <Draw/Line> 
again and draw a line like 
this. Note that the two 
end points coincide with 
the Y-axis.
[4] Trim away this 
extra segment.
[5] Trim away this 
extra segment.
48� Exercise 4. Cover Plate� �
[6] Use <Draw/Line> 
again to draw a vertical 
line and specify a 
horizontal dimension as 
shown.
[7] Trim away this 
segment.
[8] Trim away this 
segment.
[9] Trim away this 
segment.
� � Exercise 4. Cover Plate� 49
4-5 Draw Fillets
[1] Select 
<Modify/Fillet> 
and type 0.06 (in.) 
for the <Radius>.
[2] Create 6 fillets 
with the same radius 
(1-8 [2]).
[3] Create a radius 
dimension for 
anyone of the fillets 
(1-8[3]).
[4] Select 
<Modify/Fillet> 
again and type 0.15 
(in.) for the 
<Radius>.
[5] Create 4 fillets 
with the same 
radius.
50� Exercise 4. Cover Plate� �
[6] With <Modify/Fillet> 
tool still activated, create 
this fillet by clicking the 
horizontal line and the 
circle. Note that the 
horizontal line is 
automatically trimmed.
[7] Repeat the last step 
to create this fillet.
[8] Use <Draw/Line> 
to re-create the 
trimmed segment.
[9] Repeat the last step 
to re-create this line.
� � Exercise 4. Cover Plate� 51
4-6 Trim Away Unwanted Segments
[10] Use <Modify/
Fillet> to create this 
fillet (with the same 
radius as before) by 
clicking the horizontal 
line and the circle.
[11] Repeat the last step 
to create this fillet.
[1] Select <Modify/
Trim> and turn on 
<Ignore Axis>, then 
trim away this segment.
[2] And this 
segment.
[12] Create a radius 
dimension for anyone 
of the 8 fillets.
52� Exercise 4. Cover Plate� �
4-7 Extrude the Sketch to Create the Cover Plate
Wrap Up
Close DesignModeler, save the project as "Cover," and exit the 
Workbench.
[3] The final 
sketch.
[1] Extrude the sketch 
0.046 in. to create the 
cover plate.
� � Exercise 4. Cover Plate� 53
<Draw/Rectangle>
Draws a rectangle by defining two diagonally opposite points. The edges of the rectangle are either horizontal or 
vertical. To draw a rectangle at an arbitrary orientation, please use <Draw/Rectangle by 3 Points>.
<Draw/Polyline>
This tool allows you to draw a series of connected lines, called a polyline. The polyline can be closed or open. After 
defining the last point, choose <Open End> or <Closed End> from the <Context Menu>.
Auto Constraints
H� --� Horizontal
V� --� Vertical 
4-8 Review
Note:
For a comprehensive description of sketching tools, please refer to the following ANSYS on-line reference:
ANSYS Help System//DesignModeler User Guide//2D Sketching
54� Section B. Part Modeling� �
Section B
Part Modeling
As mentioned in the opening of Section A, many parts can be created by a two-step operation: drawing a 2D sketch on 
a plane and then generate a 3D body by extrusion, revolution, sweeping, or skin/lofting.
� A more complicated part often can be viewed as a series of the two-step operations; each two-step operation 
either add material to the existing body or cut material from the existing body. The exercises in Section B are 
designed to introduce the 3D modeling techniques for more complicated parts.
� � Exercise 5. Crank� 55
Exercise 5
Crank
In this exercise, we'll create a 3D solid model for a crank, of which the details are shown in the figure below. Note 
that a global coordinate system is set up and shown in the figure.
� The crank model can be viewed as a series of three two-step operations; each involves drawing a sketch on 
XYPlane and then extrude the sketch to generate a material. The materials are either add to the existing body or cut 
from the existing body.
5-1 Introduction
 Y
 X
 Unit: mm.
 7
5
 65
 Y
 Z
 20
 8
 R22
 D30
 D20
 R10
 2 ×R10
 2 ×D10
56� Exercise 5. Crank
[2] Double-click 
<Geometry> cell to start 
up DesignModeler.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
5-2 Start Up DesignModeler
5-3 Draw a Sketch on XYPlane
[1] On XYPlane, draw 5 
circles and 4 tangent lines 
(using <Draw/Line by 2 
Tangents>) like this. 
Specify the dimensions.
[3] Select 
<Millimeter> as the 
length unit.
� � Exercise 5. Crank� 57
[2] Use <Modify/
Fillet> to draw a fillet 
with a radius of 10 
mm.
[3] Trim away these 
three arc segments.
58� Exercise 5. Crank
5-4 Extrude to Create a Solid Body
[3] Click 
<Extrude>.
[4] It automatically 
switches to 
<Modeling Mode>.
[1] The active 
plane.
[2] The active 
sketch.
[6] Click <Apply>. 
The active sketch is 
automatically taken 
for <Geometry>. 
[7] Type 8 (mm) for 
<Depth>.
[9] Click 
<Generate>. 
[8] Click the 
small cyan 
sphere to rotate 
the view into an 
isometric view. 
[10] Click 
<Display Plane> 
to turn off the 
plane display.
[12] Click all the 
plus signs <+> to 
expand the model 
tree.
[11] The <Tree 
Outline> displays a 
tree structure for the 
geometry model, 
called <Model Tree>.
[13] Under the 
XYPlane, we've 
created a sketch 
(Sketch1)
[14] The 
<Extrude1> uses 
<Sketch1> as the 
base geometry.
[5] An <Extrude1> 
object is inserted in 
the model tree.
[15] This is the 
body we've 
created so far.
� � Exercise 5. Crank� 59
5-5 Create a New Sketch on XYPlane
[3] Click to switch 
to <Sketching 
Mode>.
[2] A new sketch (Sketch2) is created. Note that, for the first 
sketch of a plane, you don't need to explicitly click <New 
Sketch>. However, for additional sketches on the same plane, 
you need to click <New Sketch>. Remember that the 
drawing entities always belong to the active sketch.
[4] Click <Look At 
Face/Plane/
Sketch>.
[5] Click <Display 
Model> to turn off 
the solid model 
display.
[6] Draw a circle with a diameter 
of 30 mm. This is the only entity 
in <Sketch2>. Note that both 
Sketch1 and Sketch2 are on the 
same plane (XYPlane).
[1] Click <New 
Sketch>.
60� Exercise 5. Crank
5-6 Add Material to the Existing Body
[1] Click 
<Extrude>.
[2] Click 
<Apply>.
[3] Type 20 
(mm).[5] Click 
<Generate>.
[6] The newly created 
material is simply a 
cylinder; it adds to the 
existing body to form a 
single body.
[4] The default 
<Operation> is <Add 
Material>.
[8] Click the 
plus sign <+> to 
expand 
<Extrude2>.
[9] <Extrude2> 
uses <Sketch2> as 
the base 
geometry. The 
<Extrude2> is 
simply a cylinder.
[10] The body 
after adding 
material.
[7] <Sketch2> is 
added under 
XYPlane.
� � Exercise 5. Crank� 61
5-7 Create Another New Sketch on XYPlane
[3] Click to switch 
to <SketchingMode>.
[2] A new sketch 
(Sketch3) is created. [4] Click <Look At 
Face/Plane/
Sketch>.
[5] Click <Display 
Model> to turn off 
the solid model 
display.
[6] Draw a circle with a 
diameter of 20 mm. This is the 
only entity in <Sketch3>. Note 
that all three sketches are on 
the same plane (XYPlane).
[1] Click <New 
Sketch>.
62� Exercise 5. Crank
5-8 Extrude to Create a Third Simple Body
Wrap Up
Close DesignModeler, save the project as "Crank," and exit the 
Workbench.
[1] Click 
<Extrude>.
[2] Click 
<Apply>.
[4] Select 
<Through All>.
[5] Click 
<Generate>.
[6] The newly created 
material is simply a 
cylinder; The material 
is cut from the 
existing body.
[3] Select <Cut 
Material>.
[10] The body 
after cutting 
material.
[7] <Sketch3> is 
added under 
XYPlane.
[9] <Extrude3> 
uses <Sketch3> as 
the base 
geometry. The 
<Extrude3> is 
simply a cylinder.
[8] Click the 
plus sign <+> to 
expand 
<Extrude3>.
� � Exercise 5. Crank� 63
<Plane> and <Sketch>
A sketch must be created on a plane; each plane, however, may contain multiple sketches. In the beginning of a 
DesignModeler session, three planes are automatically created: XYPlane, YZPlane, and ZXPlane. You can create new 
planes and new sketches as many as needed.
<Active Plane> and <Active Sketch>
The currently active plane and active sketch are shown in the toolbar (5-4[1, 2]). New sketches are created on the 
active plane, and new drawing entities are created on the active sketch. You may change the active plane or active 
sketch by selection from the pull-down list, or simply clicking the names on the model tree.
Modeling Mode
In the modeling mode (5-4[4]), several modeling tools become available, including Extrude, Revolve, Sweep, Skin/Loft, 
Thin/Surface, Blend, Chamfer, Point, etc. In addition, a <Tree Outline> is displayed.
Model Tree
<Tree Outline> (5-4[11]) contains an outline of the model tree, the data structure of the geometric model. Each branch 
of the tree is called an object, which may contain one or more objects. At the bottom of the model tree is a part 
branch, which is the only object that will be exported to <Mechanical>. By right-clicking an object and selecting a tool 
from the context menu, you can operate on the object, such as delete, rename, duplicate, etc.
� The order of the objects is relevant. <DesignModeler> renders the geometry according to the order of objects 
in the model tree. New objects are normally added one after another. If you want to insert a new object BEFORE an 
existing object, right-click the existing object and select <Insert/...> from the context menu. After insertion, 
<DesignModeler> will re-render the geometry.
<Add Material> and <Cut Material>
With <Add Material> operation mode, the created material adds to the existing active body (i.e., they form a union). 
With <Cut Material> operation mode, the material is cut from the existing active body. An active body is one that is 
not frozen (to be defined later).
5-9 Review
64� Exercise 6. Geneva Gear Index� �
Exercise 6
Geneva Gear Index
In this exercise, we'll create a 3D solid model for a Geneva gear index, of which the details are shown in the figure 
below. Note that a global coordinate system is set up and shown in the figure.
6-1 Introduction
 Y
 X
 Unit: in.
 Y
 Z
 0.25
 D0.5
 0.44
 D0.25
 D1.25
 D2.47
 5 × 0.2 5 ×R0.63
 1.5
29
� � Exercise 6. Geneva Gear Index� 65
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select <Inch> as 
the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
6-2 Start Up DesignModeler
6-3 Draw a Sketch on XYPlane
[1] On XYPlane, use 
<Draw/Arc by Center> to 
draw an arc centered at 
the origin and with a radius 
of 1.235 (in.) like this.
[2] draw two lines, each 
connects the origin to an 
end point of the arc.
[3] Specify an angle 
dimension of 72 
(degrees) for the 
sector.
[4] Use <Draw/Arc by 
Center> to draw another 
arc with a radius of 0.625 
(in.) like this.
[5] draw two circles 
centered at end points 
of the new arc and 
with the same radius 
of 0.1 (in.).
66� Exercise 6. Geneva Gear Index� �
[8] Apply a 
<Constraints/Tangent> 
on the lower circle and 
the horizontal line.
[7] Draw a line connecting the upper 
circle to the outer arc like this. The 
line is parallel to the adjacent line, 
therefore make sure a <//> 
(indicating parallel auto constraint) 
appears before clicking.
[9] Apply a <Constraints/
Tangent> on the upper 
circle and the parallel line.
[6] Draw a line connecting the lower 
circle to the outer arc like this. The 
line is horizontal, therefore make 
sure an <H> appears before clicking.
� � Exercise 6. Geneva Gear Index� 67
[10] Draw a line starting from 
the origin like this. Then, make 
the outer arc symmetric about 
the newly created line. To do 
this, select <Constraints/
Symmetric>, and then 
subsequently click the line and 
the two end points of the arc.
[11] Use <Dimension/
General> to specify a 
length dimension of 
1.529 (in.).
[12] Use <Draw/Arc by 
Center> to draw an arc 
centered at one end of the 
new line. Specify the radius 
dimension of 0.63 (in.).
68� Exercise 6. Geneva Gear Index� �
6-4 Extrude to Generate 1/5 of the Gear Index
[1] Extrude the 
sketch 0.25 in.
[13] Trim away unwanted 
segments. This is the sketch 
after trimming. Note that, 
although the the sketch is no 
more blue-colored, all the 
dimensions are not changed.
� � Exercise 6. Geneva Gear Index� 69
6-5 Duplicate the Body Circularly
[1] Select <Create/
Pattern> from the 
pull-down menu.
[2] In the <Details 
View>, select 
<Circular> for 
<Pattern Type>.
[3] Click the yellow area 
to bring up <Apply/
Cancel> buttons.
[4] Select the 
body.
[5] And click 
<Apply>.
[6] Click the yellow area 
to bring up <Apply/
Cancel> buttons.
[7] Select this 
edge.
[8] And click 
<Apply>.
[9] Type 4 for 
<Copies>.
[10] Click 
<Generate>.
70� Exercise 6. Geneva Gear Index� �
6-6 Create the Hub
[1] Select <Create/
Primitive/Cylinder> from 
the pull-down menu.
[4] Click 
<Generate>.
[2] Type 0.44 (in.) for 
the <Axis Z 
Component>.
[3] Type 0.25 (in.) for 
the <Radius>.
[5] Select <Create/
Primitive/Cylinder> again.
[7] Type 0.44 (in.) for 
the <Axis Z 
Component>.
[8] Type 0.125 
(in.) for the 
<Radius>.
[6] Select <Cut 
Material> for 
<Operation>. 
[9] Click 
<Generate>.
Wrap Up
Close DesignModeler, save the project as 
"Geneva," and exit the Workbench.
� � Exercise 6. Geneva Gear Index� 71
Auto Constraints: <//>
It is applicable to a line, indicating that the line is parallel to another line in the same plane (6-3[7]).
Sketching Tools: <Constraints/Tangent>
It can be applied on two edges (lines or curves), one of them must be a curve, to make them tangent to each other 
(6-3[8, 9]). 
<Create/Pattern>
This tool allows you to create copies bodies in three types of pattern: Linear, Circular, and Rectangular (6-5).
<Create/Primitive/Cylinder>
This tool creates a cylinder by specifying its origin, axis, and radius (6-6). The origin and axis are defined by referring to 
the active plane coordinate system (1-12).
6-7 Review
72� Exercise 7. Yoke� �
Exercise 7
Yoke
The yoke is a part of a universal joint [1]. In this exercise, we'll create a 3D 
solid model for the yoke, of which the details are shown in the multiview 
drawings below. Note that a global coordinate system is also shown in the 
figure.
7-1 Introduction
 Y
 X
 Unit: in.
 Y
 Z
 R1.00
 X
 Z
 D0.75D1.20
 2 × 0.75
 R1.00
 1.
50
 3
.5
5
[1] The yoke is a part 
of a universal joint.
� � Exercise 7. Yoke� 73
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select <Inch> as 
the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
7-2 Start Up DesignModeler
7-3 Create a U-Shape Body
[1] On XYPlane, use <Draw/
Arc by Center> tool to draw 
two concentric arcs. Specify 
the radius dimensions (1.00 in. 
and 1.75 in. respectively).[2] Use <Draw/
Polyline> tool to draw 
a 3-segment polyline, 
starting from this 
point.
[5] Click the last point and 
then select <Open End> from 
the <Context Menu>. If the 
last segment is not vertical, 
use <Constraints/Vertical> to 
make it vertical.
[3] Click the second 
point. Make sure the 
first segment is vertical.
[4] Click the third 
point. Make sure the 
second segment is 
horizontal.
[6] Use 
<Dimensions/
General> to 
specify a length of 
2.50 (in.).
74� Exercise 7. Yoke� �
[7] Draw two 
vertical lines.
[8] Trim away this 
segment.
[9] Click 
<Extrude>.
[12] Click 
<Generate>.
[10] Select <Both 
- Symmetric>.
[11] Type 1 (in.) for 
<Depth>. Note that, 
the sketch is extruded 
by 1.0 in. for both 
sides of XYPlane, 
therefore the total 
depth is 2.0 in.
� � Exercise 7. Yoke� 75
7-4 Create Rounds
7-5 Create Holes
[1] Select <Blend/
Fixed Radius> 
from the toolbar.
[2] Control-
select these 4 
edges.
[3] Click 
<Apply>.
[4] Type 1 (in.) 
for <Radius>. [5] Click 
<Generate>.
[1] Select <Create/
Primitive/Cylinder> from 
the pull-down menu.
[3] Click 
<Generate>.
[2] Click to bring up 
<Apply/Cancel> buttons, 
then select <YZPlane> 
from the model tree and 
click <Apply>. Now the 
global Y-axis becomes local 
X-axis, and the global Z-
axis becomes local Y-axis. 
The origin and the axis are 
defined using the local 
(plane) coordinate system.
76� Exercise 7. Yoke� �
7-6 Create Shaft
[1] Click <New Plane> 
to create a new plane.
[2] A new plane 
(Plane4) is inserted into 
the model tree.
[3] Click to bring up <Apply/Cancel> 
buttons, then select <ZXPlane> from the 
model tree and click <Apply>. Now the 
global Z-axis becomes local X-axis, and the 
global X-axis becomes local Y-axis.
[4] Select <Offset Z> for 
<Transform 1>. Note that 
it refers to the local Z-axis.
[5] Type 3.55 (in.) 
for <Value>.
[6] Click 
<Generate>.
[7] The new plane 
become active plane.
[8] The global 
coordinate system. 
Note that the 
Workbench uses RGB 
colors to represent 
XYZ axes respectively.
[9] The local coordinate 
system of the new plane. 
Note that, in a local 
coordinate system, the 
Workbench also uses 
RGB colors to represent 
XYZ axes respectively.
� � Exercise 7. Yoke� 77
[1] Click to switch 
to the <Sketching 
Mode>.
[2] Click to look at 
<Plane4>.
[3] Click to turn off 
model display.
[4] Draw a circle 
with a diameter of 
1.2 (in.).
[5] Click 
<Extrude>.
[8] Click 
<Generate>.
[6] Select 
<Reversed> for 
<Direction>. Now, 
the extrusion 
direction is the -Z 
direction.
[7] Select <To 
Next>. Now the 
sketch will be 
extruded up to the 
next face.
Wrap Up
Close DesignModeler, save the project as "Yoke," and exit the Workbench.
78� Exercise 7. Yoke� �
Extrude Direction
There are four options you can choose for the extrusion direction: <Normal>, <Reversed>, <Both -- Symmetric>, and 
<Both -- Asymmetric>. In <Normal> case, the extrusion direction is the Z-direction of the sketching plane. When 
<Reversed> is selected, the extrusion direction reverses to the -Z-direction (7-6[6]). For <Both -- Symmetric>, the 
extrusion is along both +Z and -Z directions with the same depth (defined by <Depth>) (7-3[10]). For <Both -- 
Asymmetric>, the extrusion is along both +Z and -Z directions with the different depths (defined by <Depth> and 
<Depth 2>).
<Blend/Fixed Radius>
This tool can be used to place rounds or fillets on a body (7-4). The fillets are specified on edges, while the rounds 
can be specified on edges or faces. When faces are specified for rounds, the rounds are placed on the enclosing edges.
Create New Planes from Existing Planes
There are many ways to create a new plane [1]. Creating new plane from an existing plane (7-6[1-9]) involves 
selecting the existing plane and then transforming the existing plane to a new position and orientation.
7-7 Review
[1] There are 
many ways to 
create a plane.
� � Exercise 8. Support� 79
 0.375
[1] The support is a 
part of a clamping 
mechanism. 
Exercise 8
Support
The support is a part of the clamping 
mechanism mentioned in Exercise 1 [1]. In 
this exercise, we'll create a 3D solid model 
for the support, of which the details are 
shown in the multiview drawings below. 
Note that a global coordinate system is also 
shown in the figure.
8-1 Introduction
 Y
 X
 Unit: in.
 Y
 Z
 X
 Z
 6 ×D0.25
 2.500
 R0.313
 0
.8
75
 1.250
 2 ×R0.100
 1.
25
0
 0
.7
50
 R0.100
 0
.6
25 
0.125
 0.375
 0.125
 0.250 0.219
 1.250
 0.375
 0.250
 0.375
 Slope: 45 �
 R0.156
 1.000
80� Exercise 8. Support
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select <Inch> as 
the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
8-2 Start Up DesignModeler
8-3 Create Vertical Plate
[1] On XYPlane, draw 
three circles of the same 
radius. Specify their 
locations (two horizontal 
dimension of 1.25 and one 
vertical dimension of 1.25)
[2] Specify a 
diameter of 0.25 
in. for any one of 
the circles.
[3] Use <Draw/
Polyline> to draw a 
polyline starting 
from roughly here.
[4] Click the second 
point, making sure 
the last segment is 
vertical.
[5] Click the third 
point, making sure 
the last segment is 
horizontal.
[6] Click the fourth 
point, making sure the 
last segment is vertical. 
Then select <Closed 
End> from the 
<Context Menu>.
[7] Specify all dimensions so that all entities 
become blue-colored: length dimensions of 
2.50 and 0.625; a horizontal dimension of 
0.375, a vertical dimension of 0.875, and an 
angle dimension of 45 degrees.
� � Exercise 8. Support� 81
[8] Draw two more circles, 
specify their radii (0.156 and 
0.313) and locations 
(horizontal dimensions of 
0.219 and 0.250; vertical 
dimensions of 0.25 and 0.75) 
[9] Trim away 
unwanted 
segments.
82� Exercise 8. Support
[10] Draw two 
fillets with the 
same radius of 
0.1 in.
[13] Click 
<Generate>.
[11] Click 
<Extrude>.
[12] Type 0.125 (in.) 
for <Depth>.
� � Exercise 8. Support� 83
8-4 Create Horizontal Plate
[1] Click <New 
Plane>.
[4] Click the 
yellow area to 
bring up <Apply/
Cancel> buttons.
[2] Select 
<From Face>.
[6] Click <Apply>.
[7] Click <Generate>; 
a <Plane4> is created.
[5] Click this face at a 
location near this circle. A 
plane coordinate system 
shows up like this (the X 
axis points to global -X 
axis). Note that the 
location you click 
determines the origin and 
the axes of the plane 
coordinate system. If the 
coordinate system is not 
like this, simply re-click 
again until it is correct.
[8] Click to switch to 
<Sketching Mode>.
[9] Click to look at 
<Plane4>.
[10] Click to turn 
of the model 
display.
[11] This is <Plane4>; it 
is called an <Outline 
Plane> since it includes 
an outline. The outline 
is not part of a sketch 
but can be used as 
references.
[12] Draw a rectangle like this. Note that 
three sides of the rectanglecoincide with plane's 
outline. Specify a length dimension of 0.125 in. 
so that the rectangle become blue-colored.
[3] The default 
<Subtype> is 
<Outline Plane>.
 X
 Y
 Z
84� Exercise 8. Support
[15] Click 
<Generate>.
[13] Click 
<Extrude>.
[14] Type 1 (in.) 
for <Depth>.
[1] Click <New 
Plane>.
8-5 Create Holes on the Horizontal Plate
[6] Click <Generate>; a 
<Plane5> is created.
[3] Click the 
yellow area to 
bring up <Apply/
Cancel> buttons.[2] Select 
<From Face>.
[5] Click <Apply>.
[4] Click this face at a location 
near this corner so that the plane 
coordinate system is like this (the 
X axis points to global X axis). 
Remember, if the coordinate 
system is not like this, simply re-
click again until it is correct.
 X
 Y
 Z
� � Exercise 8. Support� 85
[7] Click to switch 
to <Sketching 
Mode>.
[8] Click to look at 
<Plane5>.
[9] Click to turn 
of the model 
display.
[10] This is 
<Plane5>; it 
includes an 
outline.
[11] Draw three circles of the same 
diameter (0.25 in.) and specify their 
positions (horizontal dimensions of 
0375, 0.375, and 1.25; vertical 
dimensions of 0.375, 0.375, and 0.125)
[16] Click 
<Generate>.
[12] Click 
<Extrude>.
[13] Select <Cut 
Material>.
[15] Select 
<Through All>.
[14] The 
<Direction> 
automatically 
becomes 
<Reversed>.
86� Exercise 8. Support
8-6 Create the Round
[1] Select <Blend/
Fixed Radius> 
from the toolbar.
[5] Click 
<Generate>.
[2] Click this 
edge.
[3] Click <Apply>.
[4] Type 0.1 (in.) 
for <Radius>.
Wrap Up
Close DesignModeler, save the project as "Support," 
and exit the Workbench.
� � Exercise 8. Support� 87
Create New Planes From Faces
You can create a new plane from an existing face (8-4[1-7]). There are subtypes to choose: <Outline Plane> and 
<Tangent Plane>. The only difference is that a <Tangent Plane> doesn't include the outline of the face. In either 
subtype, the plane coordinate system is determined according to how you click the face. The origin is usually located 
at the closest corner point or the center of a circle (or an arc); The Z-axis always points out of the face; The X-axis is 
usually parallel to the closest edge.
� An outline plane include the outline of the face (8-4[11]). The outline is not part of a sketch but can be used as 
references (datum). Without the outline, the only references are two exes (X-axis and Y-axis of the plane). However, 
you can copy the outline (or part of the outline) into a sketch, using the sketching tool <Modify/Duplicate>.
8-7 Review
88� Exercise 8a. Structural Analysis of the Support� �
[2] This is the deformed 
structure under the design 
loads. The wireframe is the 
underformed configuration.
Appendix:
Exercise 8a
Structural Analysis of the Support
In this exercise, we will perform a static 
structural analysis for the support created 
in Exercise 8. The objective is to find the 
deformation and the stresses under the 
working loads, and make sure the stresses 
are within the allowable level (30,000 psi).
� As mentioned in Exercise 1a, the 
clamping mechanism is entirely made of 
steel and is designed to withstand a 
clamping force of 450 lbf [1]. After a 
structural analysis of the entire 
mechanism [2] (which is performed in 
Exercise 17a), the results show shows 
that, to withstand a clamping force of 450 
lbf, the support is subject to external 
forces as shown [3] (also see 17a-4). 
Note that the holes on the horizontal 
plates are fixed to the ground [4].
� The analysis task will be carried out 
with <Mechanical>.
8a-1 Introduction
[1] The clamping mechanism 
is designed to withstand a 
clamping force of 450 lbf.
 62 lbf
 163 lbf
 380 lbf
[3] The external 
force on the arm. 
See 17a-14.
 380 lbf
[4] The horizontal 
plates are fixed to 
the ground.
� � Exercise 8a. Structural Analysis of the Support� 89
[2] Open the project 
"Support," which was saved in 
Exercise 8.
[1] Launch ANSYS 
Workbench.
8a-2 Start Up <Mechanical>
[3] Double-click to create 
a <Static Structural> 
analysis system.
[4] Drag <Geometry>...
[5] And drop here. A link 
is created, indicating that 
both <Geometry> share 
the same data.
[6] Double-click to 
start up the 
<Mechanical>.
90� Exercise 8a. Structural Analysis of the Support� �
[7] Make sure the length 
unit is <in.> (1a-2[8, 9]).
8a-3 Specify Loads
[1] Click to highlight 
<Static Structural>.
[2] Select <Loads/
Force>.
[3] Select this 
cylindrical face.
[4] Click <Apply>.
[5] Select <Components>.
[6] Type -380 (lbf) for <X 
Component>, and 62 (lbf) 
for <Y Component>.
� � Exercise 8a. Structural Analysis of the Support� 91
[7] Select <Loads/
Force> again.
[8] Select this 
cylindrical face.
[9] Click 
<Apply>.
[10] Select <Components>.
[11] Type 380 (lbf) for <X 
Component>, and 163 (lbf) 
for <Y Component>.
[1] Select <Supports/
Frictionless Support>.
[2] Control-select 
the three cylindrical 
faces on the 
horizontal plate.
8a-4 Specify Supports
[3] And 
control-select 
this face.
92� Exercise 8a. Structural Analysis of the Support� �
8a-5 Insert Result Objects
[1] Click to highlight 
<Solution>.
[3] A solution object is 
inserted under the 
<Solution> branch.
[2] Select <Stress/
Equivalent (von-Mises)>.
[4] Click <Apply>. 
Totally 5 faces are set to 
<Frictionless Support>.
[5] Select <Supports/
Displacement.
[6] Control-select the 
four cylindrical faces on 
the vertical plate.
[7] Click 
<Apply>.
[8] Type 0 
(in.) for <Z 
Component>.
� � Exercise 8a. Structural Analysis of the Support� 93
8a-6 Solve the Model
[1] Click <Solve>.
[4] Click <Play> to 
animate the 
deformation.
[5] Click <Stop> to 
stop the animation.
[3] The maximum 
stress is 20,608 psi, 
well below the 
allowable stress 
(30,000 psi).
[2] Select <Edges/
Show Undeformed 
WireFrame>.
Wrap Up
Close <Mechanical>, save the project as "Support-a," and exit the 
Workbench.
94� Exercise 9. Wheel� �
Exercise 9
Wheel
The main purpose of this exercise is to introduce another modeling tool (than <Extrude>): <Revolve>, which takes a 
sketch as the profile and revolves about an axis to create a 3D solid body.
� We'll create a 3D solid model for a wheel, of which the details are shown in the multiview drawings below. A 
global coordinate system is also shown in the figure.
� Note that the wheel is axisymmetric. An axisymmetric body can be created by drawing a profile then revolting 
about its axis to generate the 3D solid body.
9-1 Introduction
 X
 Unit: in.
 Y
 Z
 D4.00
 Y
 0.25
 0.50
 0.75
 45
�
 D3.50
 D1.50
 D1.00
� � Exercise 9. Wheel� 95
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select <Inch> as 
the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
9-2 Start Up DesignModeler
9-3 Create the Profile
[2] and ending here. 
Select <Open End> 
from the context 
menu. Specify all 
dimensions as shown.
[1] On XYPlane, use 
<Draw/Polyline> to 
draw a polyline starting 
from here.
96� Exercise 9. Wheel� �
[3] Use <Modify/Replicate> to 
"mirror copy" everything about the 
Y-axis. The procedure is as follows:
(a) select all segments;
(b) select <End/Use Plane Origin as 
Handle> from the context menu;
(c) select <Flip Horizontal> from 
the context menu;
(d) select <Paste at Plane Origin> 
from the context menu;
(e) finally select <End> from the 
context menu (or press <Esc>).
� � Exercise 9. Wheel� 97
9-4 Revolve the Sketch about X-Axis
[4] On the graphicswindow, select the X-axis 
and click <Apply>.
[1] Click <Revolve> in 
the toolbar.
[2] Rotate to an 
isometric view.
[5] Click 
<Generate>.
[6] Click to turn 
off the plane 
display.
Wrap Up
Close DesignModeler, save the project as "Wheel," and exit the Workbench.
[3] Click <Apply>. The active 
sketch is automatically taken 
as the profile.
9-5 Review
Modeling Tool <Revolve>
It takes a sketch as the profile and revolves about an axis to create a 3D solid body (9-4[1-5]). The angle of revolution 
can be specified.
98� Exercise 10. Transition Pipe� �
Exercise 10
Transition Pipe
10-1 Introduction
 Y
 Z
 Y
 Unit: in.
 8 ×D0.25
 2 ×D2.50
 2 ×D3.50
 2 × 0.25
 R2.50
 X
 D1.00
 R3.50
The transition pipe is used to connect two pipe segments. In this exercise, we'll create a 3D solid model for the 
transition pipe, of which the details are shown in the multiview drawings below. A global coordinate system is also 
shown in the figure.
� The main purpose of this exercise is to introduce another modeling tool: <Sweep>, which takes a sketch as the 
path and another sketch as the profile; the profile then "sweeps" along the path to create a 3D solid body.
� Note that it is possible to create the curved pipe by using of <Revolve> tool (Exercise 9), however, as an 
exercise, we decide to create the curved pipe by using <Sweep>. 
 R1/8"
 R1/16"
� � Exercise 10. Transition Pipe� 99
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select <Inch> as 
the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
10-2 Start Up DesignModeler
10-3 Create a Sketch for the Path
[1] On the XYPlane, draw an 
arc like this . This sketch will 
be used as the sweeping path 
of the curved pipe.
10-4 Create a Sketch for the Profile
[1] On the ZXPlane, draw two 
concentric circles like this. This 
sketch will be used as the 
profile of the curved pipe.
[1] Select 
<ZXPlane> (or 
click ZXPlane in 
the model tree).
100� Exercise 10. Transition Pipe� �
10-5 Create a Body Using <Sweep>
[1] Click 
<Sweep> on the 
<Toolbar>.
[3] Click 
<Generate>.
[2] Select <Sketch2> 
(from the model tree) 
for the <Profile> and 
select <Sketch1> (from 
the model tree) for the 
<Path>.
10-6 Create a Plane on One End of the Pipe
[1] Click <New 
Plane>.
[2] Select <From 
Face>.
[4] Click this face. Note that 
the local Z-axis (blue) points 
out of the face, and the local 
X-axis (red) points to the 
global -Z direction.
[3] Click the yellow 
color area to bring 
up <Apply/Cancel> 
buttons. [6] Click 
<Generate>.
[5] Click 
<Apply>
� � Exercise 10. Transition Pipe� 101
10-7 Create an End Plate
[1] On the new plane 
(Plane4), create a sketch like 
this (see next two steps). 
Remember to impose two 
<Symmetry> constraints to 
make the four small circles 
symmetric about X-axis and 
about Y-axis.
[2] The sketch 
includes a circle 
that overlaps with 
the inner circle of 
the plane outline.
[3] The sketch doesn't 
include this circle, which is 
the outer circle of the 
plane outline.
[6] Click 
<Generate>.
[4] Click 
<Extrude>.
[5] Select <Add 
Frozen>. This 
generates a 
separate body.
102� Exercise 10. Transition Pipe� �
10-8 Create Another End Plate by Duplication
[1] Click <New 
Plane>.
[2] Select <From 
Face>.
[3] Click the yellow 
color to bring up 
<Apply/Cancel> 
buttons.
[4] Click this face. 
Note that the local 
Z-axis (blue) points 
out of the face.
[6] Click 
<Generate>. 
<Plane5> is 
created.
[5] Click 
<Apply>.
[7] Select <Create/
Body Operation>.
[12] Click 
<Generate>.
[9] Select the 
existing end plate.
[10] Select <Plane4> 
from the model tree.
[11] Select <Plane5> 
from the model tree.
[8] Select 
<Move>.
� � Exercise 10. Transition Pipe� 103
10-9 Unite All Bodies into One Body
[1] Select <Create/
Boolean>.
[3] Control-select all 
three bodies.
[4] Click 
<Generate>.
[2] <Unite> is the 
default <Operation>.
10-10 Create Fillets
[1] Select <Blend/
Fixed Radius>.
[3] Click <Apply>.
[2] Control-
select these two 
edges.
[4] Click 
<Generate>.
104� Exercise 10. Transition Pipe� �
10-11 Create Rounds
[1] Select <Blend/
Fixed Radius>.
[3] Click <Apply>.
[2] Control-
select these two 
edges.
[4] Click 
<Generate>.
10-12 Turn Off Edges
[1] Select <View/Shaded 
Exterior> to turn off 
the edges display.
Wrap Up
Close DesignModeler, save the project as "Pipe," and exit 
the Workbench.
� � Exercise 10. Transition Pipe� 105
10-13 Review
Modeling Tool <Sweep>
The <Sweep> can be thought of a generalization of the <Extrude>. <Sweep> takes a sketch as the path and another 
sketch as the profile; the profile then "sweeps" along the path to create a 3D solid body (10-5). The <Sweep> also can 
be used to create spiral shapes, which will be demonstrated in Exercise 12.
Add Frozon
A body is either in a state of active or frozen. The default state is active. Two overlapped active bodies would 
automatically join together to form a single body. If either of them is frozen, they wouldn't join together. Therefore, 
the only way to avoid overlapped bodies joining together is to make at least one of them frozen. In 10-7, we create the 
end plate as frozen body (separating it from the curved pipe), so that, in 10-8, we can copy the end plate alone without 
the curved pipe.
<Body Operation/Move>
This tool moves a body (or a group of bodies) to another position and orientation in the same way that the source 
plane is move to coincide with the destination plane (10-8). If the <Reserve Bodies?> option is <Yes>, it essentially 
copies the bodies. This tool is useful for "assembling" parts together to form an assembly.
<Create/Boolean>
Using boolean operations, bodies can be united, intersected, and subtracted.
106� Exercise 11. C-Bar� �
 4
0
 4
0
 70
 D10
 12
0
 3
0
 20
 20
 R10
 R50
 100
Exercise 11
C-Bar
11-1 Introduction
 Y
 Z
 Y
 Unit: mm.
The C-shaped steel bar is used as a dynamometer, a device to 
measure the magnitude of a force P [1]. A strain gauge is bonded to 
the surface of a location as shown [2]. The measured strain is then 
used to calculate the force P.
� The details are shown below; a coordinate system is also 
included in the figure. In this exercise, we will create a 3D solid 
model for the C-bar. Due to the symmetry, we will create the 
upper half of the model and then complete the model by using a 
"mirror" (copy) operation.
 P
 P
[1] The C-
bar is used to 
measure a 
force P.
[2] A strain gauge 
is bonded to the 
surface here. The 
measured strain is 
used to calculate 
the force P.
 X
[3] The body has a 
thickness of 5 mm. 
everywhere.
[4] All fillets have 
radii of 3 mm.
� � Exercise 11. C-Bar� 107
[2] Double-click <Geometry> 
cell to start up the 
DesignModeler. Select 
<Millimeter> as the length unit.
[1] Launch ANSYS 
Workbench and create a 
<Geometry> system.
11-2 Start Up DesignModeler
11-3 Create a Sketch for the Path
11-4 Create a Sketch for the Profile
[1] On the XYPlane, 
draw a sketch like this.
[2] On the YZPlane, 
draw a sketch like this. 
The sketch is 
symmetric about the 
horizontal axis.
[1] Select 
<YZPlane> (or 
click YZPlane in 
the model tree).
108� Exercise 11. C-Bar� �
11-5 Create a Body Using <Sweep>
[1] Click <Sweep> 
on the <Toolbar>.
[3] Click 
<Generate>.
[2] Select <Sketch2> and 
<Sketch1> (from the model 
tree) as the <Profile> and 
<Path> respectively.
11-6 Create an Ear