Fundamental pro engineer

TATi UNIVERSITY COLLEGE
FUNDAMENTAL
OF
PRO ENGINEER
WILDFIRE 5.0
DESIGN SOLUTIONS
MOHAMAD HANIFF MOHAMAD YUSOFF
TOOL AND DIE DESIGN DEPARTMENT
FACULTY OF MANUFACTURING
ENGINEERING TECHNOLOGY

By Md. Haniff Md. Yusoff WILDFIRE 5.0 PRODUCT DESIGN
i
PREFACE
This module series was created to introduce new product designers or students in the
Engineering Design subject offered in several program at the Terengganu Advanced
Technical Institute. Basically the participant will learn the basic usage of the software on
how to create or design simple part. Then the module will continue onto more difficult
design task.
The exercises were added specifically on Basic Block Design parts. They are meant to be
user initial approach on how to understand the basic knowledge of the software.
The module does not emphasize all Pro Engineer commands but instead make use relevant
capabilities that the software has, to create a design concept. Pro Engineer is a tool in this
module. Any relevant features that the software has and can be utilize during the design
concept will be dealt in the text.
Starting with several simple block design, individuals’ product to create and then following
is a complete Bell Roller assembly. The series of lessons indicates numbering systems,
which identifies the sequences needed to follow in order to complete certain task.
Sometimes notes outside the sequence also important to read through. As the user progress
with the module, notice that some sequences are left out and assuming that the user already
understand the demands to proceed without showing how to start.
It is imperative to realize that this is not the best way of designing given products.
Designing concept is very universal and there can be lots of means and ways of creating
certain product such as the one provided in this module. It is mainly to provide an open
window for the designer or students to be able to strive themselves into design field, which
is very interesting and also demanding especially in 3D world.
This module can be made as a self-learner completely. But by having an instructor to assist
would be the best way of learning courses such as this. Included in this module is a
complete files of all part designed as a reference assuming that the participant may got lost
in the middle of the design phase. But it is advisable not to look onto the files unless are
told to do so.

WILDFIRE 5.0 PRODUCT DESIGN By Md. Haniff Md. Yusoff
ii
ACKNOWLEDGEMENTS
The inspiration for this module comes from the PTC Global Services modules, which has
brought me up to this level. Since PTC concentrates more on the software features, why not
create a module that can utilize the software into engineering course such as product
design.
I would like to thank Mr C.H. Lim and Mr. Ratnarajah, my former bosses in Grundig
Research and Development during my years of being a Product Design Engineer who has
taught me ample of knowledge in design field especially in plastic product.
Acknowledgment is also due to other companies that I’ve work with such as Mattel Tools,
MEC, and also Likom Research and Development. These four companies have provided
me great knowledge about design approach with different product background.
As always, special thanks are due to my wife, Norelizai Ilias, for tolerating my late nights
and weekends spent on this project, and to our children Aina, Sofiah, Fahim, and Adam for
their patience. Thank you for accepting my absent-minded and pre – occupied father.
To users of this module, I sincerely hope you enjoy the journey towards designing field.
Thank you.
MHMY
TATiUC.

iii
TABLE OF CONTENTS
Preface i
Acknowledgements ii
Table of Contents iii
BASIC BLOCK DESIGN
Corner Bracket 1
Corner Block 11
Guide Block 17
Base 25
Locking Base 31
Yoke 37
Pillow Block 43
Guide Bracket 49
Adapter Block 53
Separator 57
Shaft Support 61
Trunion 65
MACHINED PRODUCT
Ratchet Wheel 71
Swivel Hanger 77
Column Support 83
Flanged Coupling 91
Flanged Elbow 97
Connector 105
Offset Handwheel 115
ASSEMBLY FUNDAMENTAL
Assembly Fundamental 123
Cast Iron Bracket 125
Cast Iron Base 133
Steel Shaft 137
Cast Steel Roller 143
Bronze Bushing 145
Bell Roller Assembly 147
Appendix A
Appendix B
Appendix C
-----------------------------------0-------------------------------------

Introduction v
INTRODUCTION
PRO ENGINEER WILDFIRE
WHAT IS PRO ENGINEER?
 A suite of programs that are used in the design, analysis, and manufacturing of a
virtually unlimited range of products.
 It is a parametric, feature – based, solid modeling system.
 Feature – based:
 Create parts and assemblies by defining features like extrusions,
sweeps, cuts, holes, slots, rounds, and so on.
 Features are specified by setting values and attributes of elements
such as reference planes or surfaces, direction of creation, pattern
parameters, shape, dimensions, and others.
 Parametric:
 The physical shape of the part or assembly is driven by the values
assigned to the attributes of its features.
 Any changes will automatically propagate through the model.
 Can also relate the attributes of one feature to another.
 Solid Modeling:
 The computer model created is able to contain all the information
that a real solid object would have.
 It has a volume and therefore, if a density is provided, the mass and
inertia can be found.
 An important aspect of feature – based modeling in Pro E is the concept of
parent/child relationships.
 A change to the parent feature will potentially affect the child.

vi Introduction
HOW TO START?
 Below is the default start – up when entering into the program.
Default Start – Up Screen.
 Navigator.
 Shows the folder structure on the machine, with the current work
directory highlighted. The working directory is where Pro/E will
look for and save your files.
 Allows the user to organize folders and web sites into group of
favorites accessed using the four tabs at the top.
 Browser.
 Allows the user to launch regular web pages and, for example,
download part files from the web directly into Pro/E.
 The browser functions in the same way as normal web browsers.
 Sashes.
 Open and close Navigator and Browser screens.

Introduction vii
The Pro Engineer Screen.
 Main graphic area where most of the action will take place.
 The prompt/message window below the graphic area shows brief system messages
(including errors and warnings) during command execution. It is also where text or
numerical input is sometimes typed in response to command prompts that ask for
information (such as feature names or dimensions).
 Pull-Down Menus is basically similar function to familiar Windows commands.
 Short-cut Buttons provides immediate excess onto various commands compared to
pull-down menus.

viii Introduction
 The right side of the graphics window is also the short-cut buttons that deals most
with the developing of the solid modeling.
The top toolbar (default).
 Filter Setting helps identify only required selection during the development
process of the model.
MOUSE FUNCTION.
 Wildfire is meant to be used with a 3 – button mouse with a middle scroll wheel all
the better.
 “select”, “click”, “pick” a command or entity, this is done with the left mouse
button (LMB) unless otherwise directed.
 The functions controlling the view of the object in the graphics window are all
associated with the middle mouse button (MMB) and scroll wheel. These are the
important Spin, Pan, Zoom functions.

Introduction ix
 Some of these are used in combination with the Shift and Control keys on the
keyboard.
All dynamic view operations involve dragging the mouse. The dynamic view controls are
to display the 3D objects. When viewing 2D objects, some of the mouse functions change
slightly.
 Right mouse button (RMB) is normally to open pop – up menu for further
selections of command.
Common Pro/E mouse functions 3D.
Note:
More commands and feature of Pro Engineer Wildfire will be dealt in detail when going
into the module completely. Off course not all features all used in this module. Once you
get to know the fundamental of the software, you should be able to explore yourself more
on the software capabilities with additional references from PTC or any other sources
available.
GOOD LUCK.

x Introduction

Corner Bracket - 1 -
CORNER BRACKET
First off all you need to set your working directory so that all your design work will be
properly saved into appropriate location. Once having done that you may follow the
sequence provided for you below.
1. Create a new file name CORNER_BRACKET. Click onto an icon and you will
notice that a NEW dialog box opened as shown below.
Figure 1-1: “NEW” dialog box.

- 2 - Corner Bracket
2. After completing the above task, click OK to continue and change the unit into mm
by selecting the shown template below. Then click OK again to proceed further.
Figure 1-2: Change unit dialog box.
3. Make sure that all default datum icons are off except the datum plane icon. Below
are the relevant icons to be adapted.
Figure 1-3: Datum icons.
You will notice that on the screen, there are only three datum planes provided for you and
this is the common initial steps that you will always encounter during the design process.
First is to create a solid block using the top plane as the sketching area.
4. Select the Top plane> > placement > define > Sketch to go onto the sketching
mode.
5. Next is to click icon and start your sketching by clicking onto point 1 > point 2
> point 3 > point 4 > point 5 > point 6 and back to > point 1.
6. Drag your mouse away from point 1 and middle click to detach the line
construction. Middle click again to see the weak dimensions.
Your sketch should follow as shown in figure 1-4.

Figure 1-4: Sketched lines.
Notice that if your sketch is almost similar to the above, the provided dimension should be
as close as shown given below. When creating the lines, make sure that they are in exact
vertical and horizontal position except the last line when to detach it from the loop. Also do
not let the design intent activate the L1 symbol which indicates that you intended to create a
same length of lines. Otherwise your dimensions will be different than the one as shown in
figure 1-5.
Figure 1-5: Default dimensions sketched lines.
Do not worry about the value of the dimensions and its positions. Next we will reallocate
the dimensions and update the value according to the given specification of the corner

bracket. Assuming that your dimension position is as shown in figure 1-5 and you need to
change the dimension 69.49 to a different position.
7. Click icon and select the vertical line as shown in figure 1-5. Middle click
somewhere at the right side of the line to position the new dimension. Then click Ok
to accept the chosen sequence.
Notice that the dimension changes and positioned onto the desired location. You can do the
same sequence if the other dimension is not to your expectation.
8. Click the other dimensions by pressing it and drag them to a better location and
then released.
By having done the above, your sketch with the appropriate dimensions is as shown in
figure 1-6.
Figure 1-6: Adjusted position of dimensions.
Now you need to update the dimensions as per given by the bracket specification. To do
this, you need to select all dimensions before you change them. This is to avoid ambiguous
of values that might contradict to the sketches done earlier.
9. Middle click to active icon . Click from top left and drag until bottom right to
select all dimension and click icon to open the modify dimensions window.
Notice that all dimensions are highlighted to confirm that they are selected during the
grouping procedure.
10. Uncheck Regenerate before changing the value of the dimensions.

This is to make sure all dimensions are updated first before regeneration took place. The
dialog box is as shown in figure 1-7.
Figure 1-7: Updated dimensions.
11. Click to complete the sequence. Then click icon to go back to 3D. In the
dashboard area change the default depth value to 50mm and click to
complete.
The dashboard is shown in figure 1-8. You can also change the depth value by double
clicking the active value on the model.
Figure 1-8: Dashboard view.
By selecting an icon and choose the default orientation, your solid should look as
shown below in figure 1-9.
Figure 1-9: Solid created.

You may rotate your solid by pressing middle mouse button and drag it to any position you
desire. Next is to cut the first top portion of the block according to the given dimensions.
Make sure that the solid is at default orientation position.
12. Select insert > Extrude > placement > define and select the top surface of the
solid,> Sketch to go onto the sketching plane.
You need to add additional references before you do the sketching. This is to make sure the
line snap onto the created references.
13. Select Sketch > References and click onto the two edges shown in figure 1-10. Then
click Close.
Figure 1-10: Additional references.
14. Click icon and draw a rectangle from top left to bottom right as shown in
figure 1-11. Middle click to see the weak dimensions.
Figure 1-11: Shaded rectangle created.
Make sure that the rectangle snaps onto each sides of the block except the left vertical line.
That is why a horizontal dimension is given.

15. Change the dimension 54.93mm to 50 mm. Press middle buttons and then double
click onto the dimension and change the value. Press <enter> to proceed. Click
to continue with the next step. Click icon > Default Orientation.
At this point you will notice that the solid is added instead of removed. So you need to
change it from the dashboard area.
16. From the dashboard area, click onto icon and change the depth value to
30mm.
Figure 1-12: Remove icon on dashboard.
17. Change the direction of the cut if the arrow is showing away from the solid block.
You can click on the relevant arrow to do it. Finally click icon on the
dashboard to complete.
By selecting a default orientation, your solid should look as shown below in figure 1-13.
Figure 1-13: Solid model created.
The last process to complete the design is to cut the second small area. The same procedure
can be followed as before.
18. Select insert > Extrude > placement > define and select the top surface of the solid
as shown on figure 1-13, >Sketch. Select Sketch > References and pick two
additional edges for references as shown on figure 1-13. Click Ok > Close.

19. Click icon to change from solid to no hidden lines for easy sketching process.
figure 1-14. Press middle button and then double click on the dimension. Update
the dimension to 10mm > <enter>.
Again make sure it snaps to the reference edges. If there is more than one dimension then,
your rectangle does not snap to the created references.
21. Click icon to continue with the next step. Click icon > Default
Orientation. From the dashboard area, click onto icon and change the depth
value to 20mm > <enter>.
Figure 1-15: Arrow showing the correct direction.

22. Change the direction of the cut if the arrow is showing away from the yellow frame
block. You can click on the relevant arrow to do it. Then click icon on the
dashboard to complete. Click icon to change back to solid shading.
Finally your complete Corner Bracket should look like this:
Figure 1-16: Final Corner Bracket.
Save your final work. Click icon > <enter>.
Now you should have the basic understanding on how to create a solid protrusion and also
removing the solid area. Continue with the next solid creation to gain more experience in
designing simple solid block.
Good luck.

Notes:

Corner Block - 11 -
CORNER BLOCK
Again the initial stage is to set your working directory by presetting a folder before entering
into Wildfire program. Then the sequence to create this block is as follows:
1. Create a new file name CORNER_BLOCK. Click onto icon and you will notice
that a NEW dialog box opened.
Figure 2-1: “NEW” dialog box.

- 12 - Corner Block
2. Make sure to uncheck Use default template before clicking OK to continue. Next is
to change the unit into mm. then click OK to proceed for the next step.
Note that the sequence is the same as per the previous creation of solid block. We are
assuming that you are already familiar with the steps. Otherwise, please refer back to the
earlier section to recap.
3. Make sure that all default datum icons are off except the datum plane icon. Below
are the relevant icons to be adapted.
Figure 2-2: Datum icons.
Again this is to ease your design criteria only. If you feel comfortable with all datum icons
are active, then you may continue doing so. Sometimes too many datum icons may
complicate design creation. For this block, first we create a solid rectangle using top plane
as the sketching plane.
mode.
5. Next is to click icon and start your sketching by clicking onto the intersecting
point of the datum.
6. Pull down your mouse to the right and you will notice a rectangle has been created
as you move the mouse. Left click to detach the construction. Middle click to go to
a default icon .
Figure 2-3: Sketched rectangle.
Notice that we did not use the line construction but instead we use the rectangle icon. This
is another way of constructing simple rectangle block. Also there are only two dimensions
given because we snap the starting point on the intersecting of datum planes.

Corner Block - 13 -
Next is to update the two dimensions according to the given specifications of the corner
block.
7. Double click onto each dimension and change the horizontal value to 100mm and
the vertical value to 60mm. Press <enter> for each updated value.
8. Then click icon to go back to 3D. In the dashboard area change the default
depth value to 40mm > <enter> and click to complete.
Now is to cut the big area from the top of the block. Make sure additional edges of the
block is selected during the reference identification. From here it is good to inactive the
datum planes and change from shading to no hidden view.
solid, >Sketch. Select Sketch > References and click onto the vertical right edge
and bottom edge line of the solid block. Next click Ok > Close.
10. Sketch a rectangle shape as shown in figure 2-5. by selecting icon . Update the
dimensions shown in the figure.

- 14 - Corner Block
11. Click to continue with the next step. From the dashboard area, click onto icon
and change the depth value to 30mm.Click icon > Default Orientation to
see the 3D profile. Also click icon if the direction is away from the solid.
Figure 2-6: Remove block area.
From figure 2-6, you notice that the remove block is in the original solid and there are two
yellow arrows showing that this is a cut procedure and not protrusion. Also here you can
use the icon to flip the cutting position instead of clicking onto the yellow arrow.
12. Finally click icon on the dashboard to complete.
By selecting a default orientation with shading, your solid should look as shown below in
figure 2-7.
Next is to cut the right top portion as given in the specification. The same procedure can be
followed as before. Make sure all necessary references are identified before going to the
sketching mode.

Corner Block - 15 -
as shown on figure 2-7, >Sketch. Select Sketch > References and click onto the two
additional edges for references as shown on figure 2-7. Click Ok > Close.
figure 2-8. Update the dimension to 30mm.
16. Click icon to continue with the next step. From the dashboard area, click onto
icon and change the depth value to 10mm.
You can click on the relevant arrow to do it. Then click icon on the dashboard
to complete.
Figure 2-9: Solid shown in no hidden view.
The last process to complete the design is to cut the bottom left side of the block.

- 16 - Corner Block
as shown on figure 2-7, >Sketch. Select the relevant edges as a reference. Then
click Ok > Close. (Or double click twice to close the references).
19. Click icon and draw a rectangle from top left to bottom right on the desired
area. Update the dimension to 20mm.
20. Click icon to continue with the next step. From the dashboard area, click onto
icon and change the depth value to 20mm.
Then click icon on the dashboard to complete.
Finally your complete Corner Block should look like this:
Figure 2-10: Final Corner Block.
Save your final work. Click icon > <enter>.
Hopefully up to this point, you should have confidence in using the protrusion and cut
process. Also using default and created references helps to ease your sketching process.
Keep it up.
Notes:

Guide Block - 17 -
GUIDE BLOCK
This guide block needs additional process to complete. You need to use cut by sketching on
side walls and use different features than giving depth value. The rest of the feature
creation is basically the same as the first two blocks that you’ve encountered.
The first steps to design this block is to create a solid piece looking from the top view with
a depth of 60mm.
As a reminder, set your working directory properly before starting your design creation.
The sequence is as follows:
1. Create a new filename GUIDE_BLOCK. Uncheck the use default template to
change the unit into mm.
2. Make sure that all default datum icons are off except the datum plane icon.
mode.
point of the datum. Pull down your mouse to the right and you will notice a
rectangle has been created as you move the mouse. Left click to detach the
construction. See figure 3-1.

- 18 - Guide Block
5. Click on icon to create a slanting line and a small rectangular within the big
rectangle shape created earlier. See figure 3-2.
Figure 3-2: Additional lines sketched.
6. Next is to remove unwanted lines by clicking icon . Click at one position and
drag it across the unwanted lines and release the button. See figure 3-3.
Figure 3-3: Removed lines.
7. Do the same process to remove the right vertical line of the smaller rectangle. The
final sketch with rearrange and updated dimensions should look as shown in figure
3-4.
Figure 3-4: Final sketch complete.

Guide Block - 19 -
Now is to update all the dimensions according to the given specification from the Guide
Block.
8. Select all dimensions and click icon to update them. Make sure to uncheck the
regenerate command before updating. The value are given in the modify dimensions
dialog box shown in figure 3-5.
Figure 3-5: Dialog box.
9. Then click icon to complete the sequence. Click icon to go back to 3D. In
the dashboard area change the default depth value to 60mm and click to
complete.

- 20 - Guide Block
The next step would be to cut the big portion of the block which is on the right side. Use
the top surface of the block as the sketching plane. Always starts your next feature creation
with the block at its default orientation to avoid orientation confusion.
solid, >Sketch. Select Sketch > References and click onto the vertical right edge,
bottom horizontal edge, and slanted edge line of the solid block.
11. Next click Ok > Close. Sketch a rectangle shape as shown in figure 3-7.
and change the depth value to 40mm. Also click icon if the direction is
away from the solid.
Figure 3-8: Removed block area.
Note that there is no dimension constraint during the cutting process. This is because the
references selected are enough to justify the created rectangle. Also you notice that creating
a cutting block does not have to be the same shape as the block area to be removed.

Guide Block - 21 -
The next process is to cut the V shape using the front wall as the sketching plane.
14. Select insert > Extrude > placement > define and select the front wall of the solid
as shown on figure 3-9, >Sketch. Select Sketch > References and pick all
additional edges for references from the front wall except the bottom edge. Click
Ok > Close.
16. Open icon line to select the centerline, as shown in figure 3-10.
Figure 3-10: Choices of lines.
17. Draw a centerline going through the center of the front wall. Left click on top edge
line somewhere in the middle. Move the cursor down and left click again once the
line created is vertical. See figure 3-11.
Figure 3-11: Centerline creation.
18. Click icon to create a V shape as shown in figure 3-12.

- 22 - Guide Block
Figure 3-12: V shape lines.
From figure 3-12, notice that you need to change the position of the dimensions according
to the specification given for the Guide Block.
19. Click icon and select right vertical edge with point 1 and middle click
somewhere on top. Do the same sequence with the left vertical edge and point 2.
20. Next click both V shape lines to active the angle created. Your final dimension
should look as shown in figure 3-13.
21. If there is an extra dimension appear, click icon and pick point 1, point 2, and
centerline to make them equal divided.
Note that you can find the constraint icon by expanding the default icon as shown below in
figure 3-13.
Figure 3-13: Expanded constraints icon.
Figure 3-14: Updated dimensions.

Guide Block - 23 -
22. Update the dimensions as shown in figure 3-14 and click icon to go to the 3D
view.
Use your mouse to rotate the solid and from the dashboard, you need to change the
command of extrusion path to thru all instead of given depth. Also don’t forget about the
remove material icon.
23. Change the command from the dashboard as shown in figure 3-15.
Figure 3-15: Dashboard command.
24. Also change the direction of the cut if the arrow is showing away from the solid
block. Then click icon on the dashboard to complete.
Change your solid view to default orientation and your solid should look like this:
Figure 3-16: Solid block.
Finally is to add another V cut across the bigger V cut as shown in the specification. Same
procedure can be done here. The only different is the sketching plane will be on either side
of the side wall of the solid. Here we will choose the left side wall as the sketching plane.
Rotate the solid so that the left side wall is facing you.
25. Select insert > Extrude > placement > define and select the left side wall of the
solid, >Sketch. Select Sketch > References and pick all additional edges for
references from the left side wall except the bottom edge. Click Ok > Close.

- 24 - Guide Block
26. Draw a centerline going through the right side of the left side wall. Click icon
to create a V shape. Then update the required dimensions as shown in figure 3-17.
Figure 3-17: Update dimensions.
27. Click icon to go to the 3D view. Change the command from the dashboard as
shown in figure 3-15.
28. Also change the direction of the cut if the arrow is showing away from the solid
block. Then click icon on the dashboard to complete.
Note that the dimension for the centerline may be omitted if you add constraint of equal
divided for the triangle created.
Finally you’ve created the Guide Block and it should look like this:
Figure 3-18: Final solid block.
Save your final work.
Notes:

Base - 25 -
BASE
Base design block looks difficult to create for some users. But in fact it is not that difficult
if we study it thoroughly. Basically, what we need to do first is to create a solid block
shaped look like from x-direction with a depth only half the total value of 190mm. The rest
is adding and removing materials and with a bit of chamfering procedure which is the new
feature given here. Finally we can copy mirror the solid to create the other half of the
complete Base design.
1. Create a new filename BASE. Uncheck the use default template to change the unit
into mm.
3. Select the Front plane> > placement > define > Sketch to go onto the
sketching mode.
point of the datum. Pull up your mouse to the right and you will notice a rectangle
has been created as you move the mouse. Left click to detach the construction.
5. Click on icon to create a slanting line and remove the unwanted lines. Your
sketch should look as shown in figure 4-1.

- 26 - Base
Figure 4-1: Sketched with appropriate dimensions.
6. Rearrange your dimensions accordingly to the position given in the figure 4-1, and
update the value as indicated.
7. Click icon to go back to 3D. In the dashboard area change the default depth
value to 95mm and click to complete.
Next is to remove material using the top surface of the block as the sketching plane. Cut it
downwards until the leftover solid is 18mm as per given by the specification.
solid, >Sketch. Select Sketch > References and click onto all the necessary
references as shown in figure 4-3, click Ok > Close to go back to the sketching
mode.

Base - 27 -
9. Sketch two rectangles with all necessary dimensions given in figure 4-3.
Figure 4-3: Sketch with dimensions.
away from the solid.
From the specification given, notice that we need to add material in between the slot just
created. We can do this by creating a protrusion using one of the inner walls as the
sketching plane and protrude up to the other inner wall.
12. Select insert > Extrude > placement > define and select the Inner wall of the solid
as shown on figure 4-4, > Sketch. Select Sketch > References and click onto all
additional edges for references from the inner wall. Click Ok > Close.

- 28 - Base
14. Click icon to offset three lines from the edges of the wall. You will find this
icon when you open the edge selection icon as shown in figure 4-5.
Figure 4-5: Edge icons
15. Offset three edges by 22mm as shown below in figure 4-6.
Figure 4-6: Offset three edges by 22mm.
Be careful when key in the value. If the arrow shows away from the solid, then you need to
key in –ve value. Press <enter> on each value given.
16. Click Ok > Close to exit from the edge selection process.
17. Then click icon to select the very left edge line and the second bottom edge
line of the solid. Click Close to continue.
18. Use icon to trim all unnecessary line. Pick the line that you want to keep, and
click Ok to finish. The final sketch should look like as shown in figure 4-7.
Figure 4-7: Final sketch of protrusion.

Base - 29 -
19. Click icon to go to the 3D view. Change the command from the dashboard as
20. Select the opposite inner wall as a chosen surface. Then click icon on the
Up until now, your solid block should look like this:
Figure 4-9: Solid Block.
Now is to add chamfer onto the required edges by using chamfering feature.
21. Click icon and update the dashboard as shown below in figure 4-10.
Figure 4-10: Dashboard of chamfer.

- 30 - Base
22. Select the edge line that acquire 45 degree chamfer and then click icon on the
23. Continue doing the same procedure with the other edge and update the dashboard
as shown below in figure 4-11.
24. Select the other edge and toggle the side if needed to justify the correct side for the
angle and the distance. Then click icon on the dashboard to complete.
25. Select Edit > Feature Operation > Copy > Mirror > All feat > Dependent > Done.
Select Front datum plane and click Done to finish.
Finally the Base design is complete and should look like this:
Figure 4-12: Final Base solid.

Locking Base - 31 -
LOCKING BASE
Even though this Locking Base solid looks easy to design, you may find it intriguing at
certain aspect that some means of thinking needs to be done before actually going into it.
The area A and B are not as easy as it looks. There are various ways of tackling this
problem and one of the ways is to use the sweep cut with a pre sketch trajectory. So for this
design you will learn how to make use of sweep feature. The rest of the design is again
basic and should be an additional practice for you.
1. Create a new filename LOCKING_BASE. Uncheck the use default template to
sketching mode.
point of the datum. Pull up your mouse to the top right and you will notice a
rectangle has been created as you move the mouse. Left click to detach the
construction.
value to 60mm and change to both side icon . Click to complete.

- 32 - Locking Base
For this design, we position the Front datum plane in the middle of the solid. This is to
make use when sketching the trajectory for the cut sweep process. If your Front datum
plane is not in the middle, it is advisable for you to re position it accordingly. Your solid
block with the datum plane should look like this:
Figure 5-2: Solid Block.
Change the view from shading to No Hidden.
7. Select insert > Extrude > Placement > Define and select the top surface of the
solid, >Sketch. Select Sketch > References and pick all the necessary references as
shown in figure 5-3, click Ok > Close to go onto the sketching mode.
Figure 5-3: Sketched lines.

Locking Base - 33 -
8. Sketch two lines with all necessary dimensions given in figure 5-3.
and change the depth value to 60mm > <enter>. Also click icon if the
direction is away from the solid and toggle the yellow arrow to identify the correct
material to remove.
Figure 5-4 shows the cut that you’ve just created and the next step is to create the cut shape
of area A and B.
Figure 5-4: Cut done on the solid.
Change the view from shading to wireframe.
11. Click Insert > Sweep > Cut > Sketch Traj > Setup New > Plane and select the
Front plane. Click Okay > Default to rotate to the sketching plane.
12. Select Sketch > References and pick all additional reference line as shown in
figure 5-5 and click Ok > Close. Draw a line with the appropriate dimensions
shown.
Figure 5-5: Sketched line with additional references.
13. Click icon and select merged end > done to continue with the next step.

- 34 - Locking Base
14. Next is to click Sketch > References and select four reference lines shown in figure
5-6. You may need to use Selection Filter to select the respective edges of lines.
Figure 5-6: Additional references and two lines.
15. Create two lines joining at three intersecting points as shown in figure 5-6. Then
select icon to continue. Make sure that the arrow is showing away from the
solid.
16. Click Okay > OK to complete the sequence.
From now, your solid should look like this:
Figure 5-7: Created solid.
As you can see that using sweep cut is the best way for this feature creation. You can also
use surface cut by creating a datum curves for all four edges. This may be a bit longer than
using the sweep feature.
Finally is to cut the last two slots by using normal cutting procedures. Use the back surface
of the solid as the sketching plane. Rotate your solid so that the back surface is facing to the
screen.

Locking Base - 35 -
17. Select insert > Extrude > placement > define and select the back surface of the
solid, > Sketch. Select all the necessary references as shown in figure 5-8, click Ok
> Close to go onto the sketching mode.
Figure 5-8: Shaded cutting block and references.
18. Draw a cutting block as shown in figure 5-8.
away from the solid and if the remove material is not as per requested.
Figure 5-9: Locking Base.

- 36 - Locking Base
Notes:

Yoke - 37 -
YOKE
Yoke is one design solid where we can make use of the icon arc circle. For those who have
yet to utilize this features will have the opportunity to experience it in this design phase. It
should be straight forward as you have already overcome the much tougher design solid
previously. Also for now you should have enough experience during sketching procedure
with all required references and sketching methods.
1. Create a new filename YOKE. Uncheck the use default template to change the unit
into mm.
sketching mode.
point of the datum. Pull up your mouse to the right and you will notice a rectangle
has been created as you move the mouse. Left click to detach the construction.

- 38 - Yoke
Next is to cut a slot with a half circle using the top surface of the block as the sketching
plane.
solid, > Sketch. Select Sketch > References and pick all the references as shown in
figure 6-3, click Ok > Close to go onto the sketching mode.

Yoke - 39 -
8. Create a centerline snap onto the middle reference line. Sketch a rectangle and
make sure that it is divided equally with the centerline.
Note that to justify that your rectangle is equally divided is that you only have two weak
dimensions. Otherwise you need to draw them again. Also you can see there is an arrow
showing towards each other. This is another indication that it is equally divided. They are
part of the intent manager features.
9. Click icon to remove the vertical left line of the rectangle. Then click icon
to add a half circle joining the two lines together as shown in figure 6-4.
10. Select the top end point first and then select the bottom end point. Move the mouse
to the left so to create a half circle. Make sure the joining ends are tangent to each
other. Notice the letter T at each end. Left button to accept.
Figure 6-4: Arc creation with updated dimensions.
11. Change the locations of the dimensions as shown and update them accordingly.
away from the solid and toggle the yellow arrow to identify the correct material to
remove.
Your solid at this point should look like this:
Figure 6-5: Cut on the solid block.

- 40 - Yoke
Finally is to add material using protrusion and make use of the icon arc circle or a fillet.
Rotate the solid so that the back surface is facing to the screen.
14. Select insert > Extrude > placement > define and select the back surface of the
solid, > Sketch. Select Sketch > References and pick all four edges and Front
Datum as reference and click Ok > Close to go onto the sketching mode.
15. Create a centerline going thru the middle of the block or on Front Datum. Then
create a triangle using two lines as shown in figure 6-6.
Figure 6-6: Two lines to create a triangle.
16. Then click icon to add fillet on top of the triangle. Click near the end of both
lines and the fillet should look as shown in figure 6-7. Update the choices of
dimensions.
Figure 6-7: Fillet added on top of the triangle.
Here you must make sure that your fillet center point is exactly on the vertical centerline of
the solid block. Otherwise you will need more dimensions for your sketch and it may not
be accurate.
Next is to add a hole centered to the fillet just created.

Yoke - 41 -
17. Click icon and select the center point of the fillet and move the mouse further
away to create a circle. Update the dimension to 12mm diameter.
18. Then create a close line at the bottom of the triangle and your final sketches should
look like this:
Figure 6-8: Final sketches for protrusion.
19. Click icon to continue. Make sure the material is on the correct position.
Toggle it by using icon on the dashboard. Update the depth value to 10mm.
Figure 6-9: Final solid Yoke.

- 42 - Yoke
Notes:

Pillow Block - 43 -
PILLOW BLOCK
The reason why we are to design this block is to make use of the feature rounds. It can be
as your first steps of using such features. Unless you’ve already master most of the features
from Wildfire, then you may omit this portion of the design stage. Anyway it would still be
a good exercise to improve your basic knowledge in design field.
1. Create a new filename PILLOW_BLOCK. Uncheck the use default template to
To start, you may need to create a rectangular block first before adding up all the necessary
rounds and holes. From the specification given above, you can calculate the sufficient size
for the block. Treat it as a raw material size before going into machining process.
sketching mode. Create a centerline on both the vertical and horizontal references.
4. Next is to click icon and start your sketching by clicking in any quadrant of the
intersecting point of the datum. Pull towards opposite direction and you will notice
a rectangle has been created as you move the mouse.
5. Make sure that they are equally divided. Left click to detach the construction.
Again, to justify that you have created an equally divided rectangle is by having only two
dimensions. Also notice the arrows on each end point.
6. Update the dimensions as shown in figure 7-1.

- 44 - Pillow Block
Your present solid should look like this:
Next is to create a full round on top of the block. You can either click onto the top edges by
pressing control button when selecting the other edge. Then right click to select round
edges. Or follow the next sequence.
8. Click Insert > Round and select the top two long edges from the solid. Press
control button to select the other edge together.
9. Next click Sets from the dashboard and select full round. Then click icon to
complete the sequence.
The tricky part of this feature is when selecting the edges. Sometimes you might select the
wrong edges. All you have to do is undo the steps and reselect the correct edge.

Pillow Block - 45 -
Now your solid should look like this:
Figure 7-3: Round solid block.
To cut the sides of the solid, we can either do it one side and mirror or both sides at one
time which ever that is more convenient. For this particular exercise, we are going to do it
at one time.
10. Click icon and select Top datum plane to offset 16mm down. Key in -16mm in
the translation box from the Datum Plane dialog box as shown in figure 7-4.
Figure 7-4: Datum plane dialog box.
11. Select OK in the dialog box to complete the sequence.
We need to create a new datum plane because there is no flat surface that can be utilize as a
sketching plane for this particular feature creation. You can also offset from the bottom
surface of the solid with a value of 14mm instead.

- 46 - Pillow Block
12. Select insert > Extrude > placement > define and select DTM1, > Sketch. Select
Sketch > References and pick all edges as a reference and click Ok > Close to go
onto the sketching mode.
13. Create a rectangle shape snapped to the edges on each sides of the solid as shown
in figure 7-5. Update the dimension to 40mm.
Notice that L1 indicate that the opposite line is the same length. That is why there is only
one dimension needed to complete the sketches.
and change the depth value to thru all icons. Also click icon if the
material to remove.
Figure 7-6: Areas to be removed.

Pillow Block - 47 -
Next is to add full round on both ends of the solid. Here you can add two sets of edges to
make full rounds.
16. Click Insert > Round and select the vertical two edges from the solid. Press control
button to select the other edge together.
17. Next click Sets from the dashboard and select full round.
18. Select the opposite side edge and do the same routine. Then click icon to
Your solid should look like this:
Figure 7-7: Solid with full rounds.
19. Click icon and select the top flat surface of the solid as shown in figure 7-7.
20. From the dashboard, select placement and active click on no items from the
secondary references.
21. Select Front datum plane and press control key to select the cut edge of the solid as
Figure 7-8: Hole dashboard command.

- 48 - Pillow Block
22. In the dashboard, click the offset box for Front:F3, and change it to Align. For the
Edge: F8, update the value to 20mm.
For the other side, you can use copy feature to create the same hole or do the hole
procedure again. Here for faster solution, we will copy and mirror it.
24. Select Edit > Feature Operation > Copy > Mirror >Select > Dependent > Done.
Select the created hole > Ok and then select Right datum plane and click Done to
finish.
For the final hole, do the same procedure as before. The only different selection is the
Primary surface. It should be the side wall of the solid.
25. Click icon and select the side wall for the hole to go thru. Update the
dashboard accordingly as shown in the figure 7-9. Finally click icon on the
Figure 7-9: Hole dashboard command.
Finally we have completed the Pillow Block solid creation. Save your work.

Guide Bracket - 49 -
GUIDE BRACKET
The best way to design a solid block like this is to look at the most common shape. You
should see that the least feature creation for this is by using the y-direction as the first
sketching plane. Probably you need to be skillful enough to sketch certain shapes during
the 2D sketching mode. Using a line icon would be ideal for this shape. It will be a good
exercise for you.
Again as a reminder, set your working directory properly before starting your design
creation. The sequence is as follows:
1. Create a new filename GUIDE_BRACKET. Uncheck the use default template to
3. Select the Front plane > > placement > define > Sketch to go onto the
sketching mode.
Make sure that all relevant dimensions are identified and then use the line icon to sketch
the first shape of the block. You should by now know how to fully utilize the line icon.

- 50 - Guide Bracket
4. Select icon and sketch a shape given in figure 8-1. Make sure that the position
of the default references are followed accordingly.
Figure 8-1: Sketched shape.
The above figure shows the solid created. Notice that by choosing the correct shape to start
with may save a lot of time and features. Finally is to add cut section on top of the existing
solid. You may need to change the view to No Hidden.

Guide Bracket - 51 -
6. From figure 8-2, select the Top surface of the solid. Click icon > placement >
define > Sketch > Sketch > References and click three additional references > Ok
> Close.
7. Sketch using icon to create a cutting block as shown in figure 8-3 below.
Update the dimension as shown below.
Figure 8-3: Sketch block to cut.
and change the depth value to 20.00mm. Also click icon if the direction
is away from the solid and toggle the yellow arrow to identify the correct material
to remove.
Figure 8-4: Final solid creation.
Save your work.

- 52 - Guide Bracket
Notes:

Adapter Block - 53 -
ADAPTER BLOCK
To create this shape needs four feature creations which is one protrusion to create an initial
solid block and then three cutting features to complete. Here we will choose z-direction as
the solid protrusion. This means that our sketching plane for this is the top of the solid
block. After securing your working directory, you may proceed with the following
sequence.
1. Create a new filename ADAPTER_BLOCK. Uncheck the use default template to
mode. Sketch the shape given with dimensions in figure 9-1 below.
Figure 9-1: Sketched shape for protrusion.

- 54 - Adapter Block
value to 60mm. Click to complete.
Figure 9-2: First Solid.
Next is to cut from the z-direction or the Front surface of the solid. It is advisable that you
change the view into wireframe mode for better viewing during sketching.
5. Select the Front plane > > placement > define > Sketch > Sketch >
References > add additional reference > Ok > Close to go back to the sketching
mode.
6. Sketch a cutting block using icon with the given dimension as shown in figure
9-3 below.
Figure 9-3: Cutting block sketch.
material to remove.
8. Then click icon on the dashboard to complete.

Adapter Block - 55 -
Your solid block should be updated as shown below.
Figure 9-4: Updated Solid.
Following is to cut thru all from the x-direction or the Right sketching plane. Click icon
and choose Right to orient the solid.
9. Select the Right plane > > placement > define > Sketch > Sketch >
References > add additional reference > Ok > Close to go onto the sketching
mode.
10. Sketch a cutting block using icon with the given dimension as shown in figure
9-5 below.
Figure 9-5: Sketched Block.
material to remove.
12. Next click icon on the dashboard to complete.

- 56 - Adapter Block
Finally is to cut the top portion of the solid to complete the sequence. Click icon and
choose Top Orientation.
13. Select the Top surface of the solid shown in figure 9-4. Click icon > placement
> define > Sketch > Sketch > References > add additional reference > Ok > Close
to go back to the sketching mode.
14. Sketch by using icon line with the given dimensions shown in figure 9-6 below.
Figure 9-6: Sketched cutting block.
remove.
Your final solid should look like this.
Save your work.

Separator - 57 -
SEPARATOR
This separator is chosen because of the unique feature. To create this solid, you may need
to add datum plane to be able to add solid or even remove material from the existing solid.
Sometimes, with careful study, you may be able to create it in the best manner with less
feature creation.
Here is one ways of doing it, but may not be the best. You may follow this sequence or try
out on your own after already having gone through certain amount of training in this
module. Again make sure that your working directory is set accordingly.
1. Create a new filename SEPARATOR. Uncheck the use default template to change
the unit into mm.
3. Select the Right plane> > placement > define > change orientation to Top >
Sketch to go onto the sketching mode. Sketch the shape given with dimensions in
figure10-1 below.

- 58 - Separator
Figure 10-1: Sketched shape to protrude.
Your first solid should look like this. Make sure the position of the datum planes is set
accordingly.
Figure 10-2: Initial Solid creation.
Next is to add additional solid on top of the initial solid. Still we will use the right datum as
the sketching plane. Click icon and choose Right Orientation.

Separator - 59 -
Sketch > Sketch > References > add additional references > Ok > Close to go
back to the sketching mode. Sketch the shape given with dimensions in figure10-3
below.
Figure 10-3: Additional solid sketch.
Your updated solid should look like this.
Figure 10-4: Updated solid creation.
Finally is to cut the respective area thru all by using the Front datum plane as the sketching
plane for this purpose. Click icon and choose Front Orientation.

- 60 - Separator
mode. Sketch the shape given with dimensions in figure10-5 below.
Figure 10-5: Cutting sketch shape.
material to remove.
Save your work.

Shaft Support - 61 -
SHAFT SUPPORT
The only different between the rest of the block that you’ve encountered is that this shaft
support has a revolve feature. So it can be a good starting point to know how to make use
of the revolve feature. The rest of the feature creation is basically straight forward and you
should be able to design it yourself. But still we will provide you one of the ways to create
it and below are the steps provided.
After setting your working directory, you can proceed as follows.
1. Create a new filename SHAFT_SUPPORT. Uncheck the use default template to
The first solid creation would be the base shape of the shaft. The oblong hole can be
created together with the base shaft during sketching the shape in 2D mode.
3. Select the Top plane > > placement > define > Sketch to go onto the sketching
mode.
4. Sketch the shape of the base as shown in figure 11-1 with all the dimensions given
and constraints indicated.

- 62 - Shaft Support
Figure 11-1: Base sketched shape.
value to 8.0mm and click to complete.
Your initial solid should look like this.
Figure 11-2: Initial solid creation.
Finally is to add revolve feature to complete the sequence. Note that using revolve, the
sketch must be a close loop and must have a centerline.

Shaft Support - 63 -
mode.
7. Sketch the revolve shape as shown in figure 11-3 below.
8. To dimension in diameter format, click point1 > Centerline > point1 and middle
click to position the dimension.
9. Click point2 > Centerline > point2 and middle click to position the dimension.
Figure 11-3: Revolve sketch.
10. Next click and notice that the solid automatic creates a 360 degrees rotation as
shown below.
Figure 11-4: Revolve preview.

- 64 - Shaft Support
11. Finally click icon to accept the default and complete the sequence for this part
design.
Your final solid creation should ends up like this,
Save your work.

Trunion - 65 -
TRUNION
To design Trunion, it takes special study to see what and how the starting point should be
because it relates to symmetrical shape which should be an advantage here. If you
remember designing Base, then it is almost similar design sequence for this part.
Here it will be a good exercise for you to become truly familiar with sketching concept,
constraints and references. Following is the sequence for you to acquire to complete the
designing of this part.
Again as a reminder, set your working directory or check them to ensure that they are in
order.
1. Create a new filename TRUNION. Uncheck the use default template to change the
unit into mm.
Sketch > Ok to go onto the sketching mode. Sketch the shape given with dimensions
in figure12-1 below.

- 66 - Trunion
Figure 12-1: Protrusion sketch shape.
value to 50.0mm and change to both side icon . Click to complete.
Below is the solid that you’ve just created.
Figure 12-2: Initial solid.

Trunion - 67 -
Next is to cut from the top side of the solid and goes straight down by using thru all feature
command. Also notice that we can cut multiple areas in one time as long as the portion to
be cut is the same depth.
5. Select the Top surface (figure 12-2) > > placement > define > Sketch > Sketch
> References > add additional reference > Ok > Close to go back to the sketching
mode. Sketch the shape given with dimensions in figure12-3 below.
Figure 12-3: Sketched cut area.
Note that if you are having difficulties in defining the sketched section, may be you need to
check again your references and the position of the centerline. Also you need to add
constraints so that symmetrical sections are equally divided. Use icon to add up any
relevant constraint in your sketching mode.
material to remove.
Your current solid part should look like this,

- 68 - Trunion
Figure 12-4: Solid updated.
8. Select the Front surface (figure 12-4) > > placement > define > Sketch >
Sketch > References > add additional reference > Ok > Close to go back to the
sketching mode. Sketch the shape given with dimensions in figure12-5 below.
Figure 12-5: Sketch cut.

Trunion - 69 -
material to remove.
Finally is to mirror all geometry created and the part is complete.
11. Select Edit > Feature Operation > Copy > Mirror > All feat > Dependent > Done.
Select Front datum plane and click Done to finish.
Your final solid should look like this:
Figure 12-6: Final solid created.

- 70 - Trunion
Notes:

Ratchet Wheel - 71 -
RATCHET WHEEL
This part model is chosen due to the multiple cutting elements. We can use pattern feature
to create such a design shape in radial category. The rest of the design should be easy
enough for you to complete. For those who doesn’t have any experience in using pattern
process will find that this exercise useful. After setting your working directory, you may
follow the sequence below.
1. Create a new filename RATCHET_WHEEL. Uncheck the use default template to
sketching mode.
Figure 13-1: Sketched circle.

- 72 - Ratchet Wheel
4. Sketch a circle with a hole in the middle as shown in figure 13-1 above.
Your first solid creation should look like this.
Figure 13-2: Initial solid created.
Next is to add shaft followed with cutting a key seat.
6. Select the Front surface (figure 13-2) > > placement > define > Sketch >
Sketch > References > add additional reference > Ok > Close to go onto the
sketching mode.
7. Sketch the shaft circle as shown in figure 13-3 below.
Figure 13-3: Shaft sketched circle.

Note that protrusion is created away from the existing solid. If not then, you need to toggle
them to the opposite direction. Click icon and choose Default Orientation. Change
the view type to No Hidden.
9. Select the Top shaft surface (figure 13-4) > > placement > define > Sketch >
Sketch > References > add additional reference > Ok > Close to go onto the
sketching mode. Sketch the shape given with dimensions in figure13-5 below.
Figure 13-5: Sketched cut portion.
material to remove.
Finally is to create a cut portion at the edge of the circle block. We only need to create one
section and use pattern features to add up to 24 additional cutting edges to complete the
sequence of this part. Change the position of the solid back to Default Orientation and the
view to No Hidden unless already done.

12. Select the Front surface (figure 13-2) > > placement > define > Sketch>
Sketch > References > add additional reference > Ok > Close to go back to the
sketching mode.
13. Sketch the cut section as shown in figure 13-7.
Note that you need to add a construction line of a circle with a diameter of 130mm. Click
icon to select the circle and right click to open a dialog as shown in figure 13-6 and
choose construction line.
Figure 13-6: Dialog box.
Figure 13-7: Sketched cut portion.

material to remove.
Your current solid should look like this:
Next, make sure that axis icon is active.
16. From the model tree, click on to the last feature created as shown in figure 13-9.
Figure 13-9: Model Tree.
17. Click Edit > Pattern and update the dashboard as shown below in figure 13-10.

Figure 13-10: Pattern dashboard.
Note that once you choose Axis in the dashboard, you need to select the axis of the circle
you’ve created in the solid. Then update all necessary items in the dashboard.
Your final solid creation should ends up like this:
Save you final work.

Swivel Hanger - 77 -
SWIVEL HANGER
This product is mainly to provide you an additional practice on using the protrusion
features and also the usage of pick and place features such as rounds. Also here you don’t
have to use a hole feature but can immediately create a cut hole during the 2D sketching.
But then again, it will totally depend on what and how your design requirement is going to
be. Basically it is all up to your own means of doing the design creation.
Once you’re in the correct working directory, you may proceed as follows.
1. Create a new filename SWIVEL_HANGER. Uncheck the use default template to
Sketch > Ok to go onto the sketching mode. Sketch the shape given with dimensions
in figure14-1 below.

- 78 - Swivel Hanger
Figure 14-1: Sketched protrusion.
Your first shape of solid should look like this:
Next is to add the top round shaft. Notice that we are going to use the Right datum plane as
the sketching plane for this purpose. This is to show that you can also add protrusion inside
the solid that is already created. Set your solid to Default Orientation.

Sketch > Sketch > References > add additional references > Ok > Close to go
back to the sketching mode. Sketch the shape given with dimensions in figure14-3
below.
Figure 14-3: Added protrusion sketch.
Figure 14-4: Updated solid.
Now is to add the flat piece with two holes on each side. Make sure that you select the
appropriate references for this feature creation. Click icon and choose Bottom
Orientation.
7. Select the Bottom surface (figure 14-4) > > placement > define > Sketch >
Sketch > References > add specific reference > Ok > Close to go onto the
sketching mode.

8. Sketch the shape as shown in figure 14-5 below.
Figure 14-5: Sketched protrusion on one side.
You can use mirror in sketch feature to draw the same shape on the other side.
9. Click icon to capture all drawn sketched. Red color means that they are
selected.
10. Select icon and click onto horizontal centerline to mirror the image.
Notice the added sketch on the other side as shown below.
Figure 14-6: Mirror image of the sketch.

Your updated solid should look like this:
Be careful to either toggle the direction of solid creation so that it will protrude onto the
desired location. Click onto the yellow arrow or use icon to change the direction if
needed.
Finally is to add rounds on all required sharp edges.
12. Click icon and pick edges as shown in figure 14-7 above. Update the round
value to 6.0mm and click icon to complete.
13. Continue to do the same process onto the other required edges to complete the task.
Your final solid creation should look like this:

Notes:

By Md.Haniff Md. Yusoff WILDFIRE 5.0 PRODUCT DESIGN
Column Support - 83 -
COLUMN SUPPORT
This product is another example that can be developed using protrusion and cut features.
Also notice the center cutting section are done using a revolve cut feature. The symmetrical
of the unit also gives significant advantage to the designer to consider half shape to be
developed and mirror image them to complete the task. Here is one of the ways to develop
it. You may proceed on your own or follow the steps provided for you.
Always remember to set your working directory first before proceeding to the steps given.
1. Create a new filename COLUMN_SUPPORT. Uncheck the use default template to
mode.
4. Sketch the shape of the block as shown in figure 15-1 with all the dimensions given

- 84 - Column Support
Figure 15-1: Sketched block.
Below is the initial look of the solid with the appropriate location of the datum planes.
Change the view to Default Orientation.
Next is to cut both side of the block from the top surface.

6. From figure 15-2, select the Top surface of the solid. Click icon > placement >
define > Sketch > Sketch > References > add additional references > Ok > Close.
7. Sketch using icon to create a cutting block as shown in figure 15-3 below.
Update the dimension as shown below.
Figure 15-3: Cut sketch.
and change the depth value to 35.00mm. Also click icon if the direction
is away from the solid and toggle the yellow arrow to identify the correct material
to remove.
You may need to rotate the solid to see the cutting section more clearly.
10. From figure 15-4, select the surface of the solid. Click icon and update the
dashboard as shown below in figure 15-5.

Figure 15-5: Hole dashboard.
11. For secondary reference, pick the Front datum plane and the edge shown in figure
15-6. Press control button to add the second reference.
Figure 15-6: Element to choose from the solid.

Next is to add hole on the vertical wall of the solid from the same side.
13. From figure 15-6, select the vertical surface of the solid. Click icon and update
the dashboard as shown in figure 15-5.
14. Click icon on the dashboard to complete.
The update solid should look like this:
Now is to add steps onto both holes that you’ve created earlier. Make sure that an icon
datum axis is active.
15. Click icon > placement > pick A_2 and update the dashboard as shown below
in figure 15-8.
For the secondary reference, pick the surface as shown in figure 15-7 above.
17. Do the same process for the other hole by selecting A_4 from figure 15-7. (Your
Axis number may be different).
Note that the secondary reference should be the vertical wall that is the surface of the hole
created.

We can in fact mirror the holes that we added to the other side.
18. Select all the hole features that you’ve added from the Model tree as shown below
in figure 15-10.
Figure 15-10: Model Tree.
19. Click icon > Front datum > to complete the sequence.
Figure 15-11: Mirrored holes.
Next is to use revolve to cut the middle area of the solid. Set the view to default orientation.
Change the view to No Hidden for better viewing.

20. Click icon > placement > define > pick Top surface > Sketch > Sketch >
Reference > add additional reference > Ok > Close.
21. Sketch the shape to cut with all necessary dimensions and constraint as shown in
figure 15-12.
and make sure it is 360 degrees. Also click icon if the direction is away
from the solid and toggle the yellow arrow to identify the correct material to
remove.
Figure 15-13: Updated solid in no hidden view.

Finally is to add all necessary rounds onto the solid to finish the task.
24. Click icon > update value to 15.0mm (from the dashboard) and pick edges as
shown in figure 15-14 above. Click icon to complete.
25. Do the same process for other sharp edges with a value of 5.0mm.
Figure 15-15: Solid with added rounds.

Flanged Coupling - 91 -
FLANGED COUPLING
Here is another good exercise for you to do. It is a good practice to understand the types of
drawing information given and be able to extract necessary dimensions into the creation of
the solid part of the unit. Designing this flanged coupling makes use of the pattern features
and revolves protrusion. You will also need to sketch a diamond shape and add on to the
revolved solid creation. Final touch up would be rounds and a chamfer features.
As usual, make sure to secure your working directory before proceeding to the sequence
given.
1. Create a new filename FLANGED_COUPLING. Uncheck the use default template
to change the unit into mm.
3. Select the Right plane > > placement > define > Sketch to go onto the
sketching mode.

- 92 - Flanged Coupling
4. Sketch a revolve sketch to create the basic shape of the flange as shown below in
figure 16-1.
Figure 16-1: Revolved sketch shape.
5. Click to continue with the next step. Click icon on the dashboard to
complete.
Note that during sketching, make sure those constraints such as L1 is not added,
otherwise your dimensions will be less than what is given in figure 16-1.
Next is to add the diamond shape onto the tip of the cylinder. It is better to change the view
into no hidden for better viewing.

6. From figure 16-2, select the surface of the solid. Click icon > placement >
define > Sketch.
7. Sketch the shape of the diamond as shown in figure 16-3.
Figure 16-3: Diamond shape sketch.
Note that you need to be very careful to create the shape with relevant constraints to help
you manage the right shape. Make sure that all indicated constraints are available in your
sketch. Also the dimensions are appropriately indicated as given.
8. Click to continue with the next step. Update the depth to 12.0mm and make
sure that the creation arrow is towards the solid. If not then click icon to
toggle. Click icon on the dashboard to complete.

Now is to create one hole and then pattern it to another six similar size hole with equally
divided angle of 60 degrees. Set your view to Default Orientation.
9. From figure 16-4, select the indicated surface of the solid. Click icon >
placement > define > Sketch.
10. Create a construction diameter of 58.0mm. Add a circle with a diameter of 8.0mm
as shown in figure16-5.
Figure 16-5: Sketched hole.

and change the depth value to thru all. Also click icon if the direction is
remove.
13. Next click the hole > right click > pattern and choose axis from the dashboard as
14. Then pick axis A_2 on the solid and update the dashboard as shown in figure 16-7.
Make sure that the datum axes are active.

Finally is the chamfering and rounds to be added.
16. Click icon and update the dashboard as shown in figure 16-9.
Figure 16-9: Chamfer dashboard.
17. Next pick the edge to be chamfered as shown in figure 16-8 and click icon to
complete.
18. Click icon > update value to 2.0mm (from the dashboard) and pick edges as
shown in figure 16-8 above. Click icon to complete.
Finally your solid should end up like this:
Figure 16-10: Final solid part.
Save your work.

Flanged Elbow - 97 -
FLANGED ELBOW
Flanged elbow concept design will be on the usage of sweep feature or pipe. We can either
create the coupling disc first or the pipe. Here we will start with the right disc and then we
will add the pipe using the sweep protrusion feature.
With the correct working directory, you may follow the given sequence.
1. Create a new filename FLANGED_ELBOW. Uncheck the use default template to
sketching mode.
4. Sketch the circle with all relevant holes and constraints together with the updated
dimensions in figure 17-1.
Figure 17-1: Sketched circles.

- 98 - Flanged Elbow
Next is to sketch a trajectory curve for the sweep of the pipe. Make sure it is at Default
Orientation.
6. Select Top datum plane > > Sketch. Change your view to no hidden and
sketch the arc as shown in figure 17-3 below. Click icon and pick on the
number of sequence shown.
Figure 17-3: Sketched Arc.

7. Then click icon and select icon to update the sweep dashboard as shown
in figure 17-4.
Figure 17-4: Sweep dashboard.
8. Next click icon from the dashboard to sketch the pipe size as shown in figure
17-5.
Figure 17-5: Pipe circle size.
9. Click icon to go back to 3D and click to complete.

Now you can do the same process onto the other end of the pipe or tube to create the disc.
Use the end surface of the tube as the sketching plane. Rotate your solid and position it as
10. Select Surface (figure 17-6) > > placement > define > Front datum plane >
Sketch > Add reference > Ok > Close to go onto the sketching mode.
Note that you need to identify perpendicular reference because the position of the sketch
surface is not on the default datum plane.
Figure 17-7: Sketched disc.
11. After finishing the sketch above, click icon to go back to 3D. In the dashboard
area change the default depth value to 10.0mm and click to complete.
For the rest of the four holes, we are going to use hole feature instead as a practice. Rotate
your solid and positioned it as shown in figure 17-8.

Figure 17-8: Items to choose for hole process.
12. Click onto icon > Placement > Surface (figure 17-8) and update the value
inside the dashboard as shown in figure 17-9.

Note that you need to press control button to add the second secondary reference.
13. Then click icon to complete.
14. Select the recent hole that you’ve created, and right click > pattern > axis (from
dashboard) > pick A-15 and update the rest of the value inside the dashboard.
Your current solid should look like this:

18. Select the step hole again, right click > Pattern > .
Your step hole should add up to the other three holes that you’ve patterned earlier. The
solid should update as shown below.
Next you can add step hole for the other side of the coupling disc following the same
procedure that you did recently. Do item 12 to 14 and change the diameter to 18.0mm and
the depth to 2.0mm to complete the patterning process.
19. Finally is to add rounds R3 onto the edges shown in figure 17-13. You should be
able to do this on your own.
Below is your final solid.
Save your work.

Notes:

Connector - 105 -
CONNECTOR
Connector design phase will be using circles and ellipse as the joining part between the two
round slots. We will also use draft feature to create tapering onto both the two slots. The
initial creation and position of the datum plane is important in order to produce the best
way of designing this product.
Again if you feel that you can start on your own, you may proceed. Otherwise, below is the
sequence that you can explore as you progress. Before you proceed, make sure that you are
in the correct working directory.
1. Create a new filename CONNECTOR. Uncheck the use default template to change
the unit into mm.
mode.
4. Sketch the shape of the block as shown in figure 18-1 with all the dimensions given

- 106 - Connector
Notice that the Front datum is purposely allocated away with certain distance from the
solid creation. Next is to create the other slot on the opposite side of the Front plane. We
cannot create it together with the earlier part because the depth of protrusion is not similar.
Set your view to Default Orientation.
mode.

Connector - 107 -

- 108 - Connector
Now is to joint the two solid part with the ellipse joining shaft. Here we will use the up to
next feature in the protrusion creation. Adjust your solid back to default orientation.
sketching mode.
Select the ellipse feature creation from the toolbox as shown below in figure 18-5.
Figure 18-5: Sketch toolbox.
9. Click icon and sketch the ellipse shape as shown in figure 18-6 below.
Figure 18-6: Sketched ellipse.
10. Click icon and update the dashboard as shown below in figure 18-7.Click
Option to change to next.
Figure 18-7: Protrusion dashboard.

Connector - 109 -
11. Click to complete.
Next is to add draft angle on both of the slot with a draft angle 10 degrees splitting in the
middle. We will make use of the Top datum plane as the splitting plane.
12. Click on icon > References. Pick the outside surface of both slots. Make sure
to press Control Button when adding the surfaces.
13. In the dashboard click inside the add draft hinge box and pick Top datum plane.
14. Clicks Split and change to Split by draft hinge. Then update the draft angle to 10
degrees and toggle it the draft onto the right place.
Figure 18-9: Draft angle dashboard.
After having done this, you should be able to understand how draft feature is created. We
can also use revolve to create this shape instead of using draft.

- 110 - Connector
To add additional solid on the side of the large slot, we can use additional floating plane as
a sketching plane and protrude up to the existing solid.
16. Click icon and pick Front datum plane. In the dialog box update translation
to 75.0mm. Click Ok to close.
17. With DTM 1 still active, click icon > > placement > define > Sketch to go onto
the sketching mode.
18. Sketch the rectangle shape with given dimensions as shown in figure 18-10.
19. Next click icon > and toggle if the arrow is showing away from the solid
and click to complete.

Connector - 111 -
20. Click icon and pick both edges as shown in figure 18-11. Make sure to press
Control Button when selecting both edges.
21. From the dashboard pick Sets > Full Round > to complete.
22. Click surface (figure 18-11) > > Placement and update all necessary items
Your solid should be updated as shown below:

- 112 - Connector
Next is to add the steps on each side of the hole you’ve created earlier. You can use the
hole feature with coaxial elements in the dashboard.
26. Do the same procedure for the other side of the hole area.
27. From figure 18-13, select the Cut surface > > placement > define > Sketch >
Sketch > Reference > Add additional references > Ok > Close to go onto the
sketching mode.
Figure 18-15: Cut sketched area.

Connector - 113 -
material to remove.
Finally is to add rounds of radius R6.0mm on all necessary edges as shown in the
beginning of this exercise. You should be able to do this on your own.
Below is the final solid creation.
Save your work.

- 114 - Connector
Notes:

Offset Handwheel - 115 -
OFFSET HANDWHEEL
To create this product, you will use a sweep protrusion and pattern features in the process.
You will create the round handle first and then add a profile spoke using the sweep
features. Then we will use pattern to add four equally spaced spokes around the handle or
the handwheel. The rest of the process is basically an exercise to familiarize with the most
common feature in solid modeling.
Below is the available sequence for you to explore, but first always confirm that you are in
the correct working directory.
1. Create a new filename OFFSET_HANDWHEEL. Uncheck the use default
template to change the unit into mm.
sketching mode.

- 116 - Offset Handwheel
4. Sketch the shape shown in figure 19-1 with all the dimensions given and constraints
indicated.
Next we will add the slot cut. Set your view to Default Orientation.
6. Select the Right plane > > placement > define > Sketch > Sketch >
References > Add additional reference > Ok > Close to go onto the sketching
mode.
Figure 19-3: Sketched slot.

7. Click icon and update all necessary items inside the dashboard as shown in
figure 19-4.
Figure 19-4: Cut dashboard.
Now we can add the wheel as our next sequence. Here we are going to sketch a curve first
as a sweep trajectory. Then we will use the sweep features to create the wheel. Set at
Default Orientation.
9. Click icon to add offset datum from the front surface by 42.0mm.Refer to
figure 19-6.

Figure 19-6: Offset Datum plane.
If the datum plane is on the opposite side, you can click and drag it to the other side as
shown in figure 19-6 above.
10. Click OK to accept the choices.
11. With DTM1 still active click icon > Sketch to go to the sketching plane. Sketch
the circle as shown below in figure 19-7.
Figure 19-7: Sketched curve.
12. Click icon to continue. Click icon > > and add a circle with
diameter 26.0mm as shown in figure 19-8.

Figure 19-8: Sketched circle for the wheel.
13. Finally click icon and to complete.
Your updated solid is as shown:
Next is to add the first spokes by creating the trajectory and continue sketching the profile
of the spokes to sweep through it.
14. Select the Right plane > > Sketch > Sketch > References > Add additional
references > Ok > Close to go to the sketching plane.
15. Sketch the curve as shown in figure 19-10.
Figure 19-10: Sketched curve.

16. Then click icon to continue. Click icon > > and add a profile for
the spokes as shown in figure 19-11.
Figure 19-11: Sketched spokes profile.
Note that the starting position of the sketching plane can be either end of the trajectory
curve.
17. Click icon to continue. Update all necessary items in the dashboard shown
below in figure 19-12.
Figure 19-12: Sweep dashboard.
Your update solid should look like this:

19. Pick the spoke that you’ve created and click icon > Axis > pick A_3 and check
the rest of the items in the dashboard as shown in figure 19-14.

21. Click icon and update the radius to 3.0mm in the dashboard. Pick all
necessary sharp edges to add rounds.
22. Finally click icon to complete the task.
Your final solid Offset Handwheel should look like this:
Save your work.
Notes:

Assembly Fundamental - 123 -
ASSEMBLY FUNDAMENTAL
Assembly process can be easily assembled when all relevant references provided are in line
and fits to all necessary requirements given when designing each part separately. It is truly
important that the given specifications are vividly correct before pursuing the design
process. Otherwise the assembly of the components will be incorrect and will leads to time
wastage and efforts.
Assembly can be done after all relevant components are developed first, then each
components will be assembled one by one to compose as an assembly product.
Alternatively, components of an assembly product can be designed and developed in
assembly mode whereby all relevant references are determined during the development of
the product itself. This method is mainly for a much tougher product assembly. When
dealing with a simple assembly product such as the Bell Roller Assembly parts, such
components can be designed and developed separately and assembled at the end of the
design process.
Here, we will start with designing each component of the Bell Roller product. Then we will
assemble them together to produce the assembly required. To do this, we need to confirm
the references needed before designing them, for instance, the Roller part must be design
with the axis of revolution exactly symmetrical to the part itself. Also the Shaft part needs

- 124 - Assembly Fundamental
to be developed with a plane divided equally so that those references can be used as part of
the assembly utilities. Otherwise, you may encounter some difficulties during assembly
procedure without having appropriate references. New reference may need to be added just
to fulfill the basic requirement of assembly procedure which is definitely a waste of time
and effort.
Designing product needs a lot of patience and stringent focus onto the issue of the part or
parts to be developed. Composition of components into developing a new product needs a
head on thinking of how or what would be the best way of combining such designed
methods so that the complete assembly of the product would be the best solution achieved.
Probably by having rough sketches on various selections of methods for assembly would
definitely help to justify the best possible solution for any designed product especially
assembled parts.
As a starting point for intervening into assembly process, this Bell Roller product design
will help the user to understand the basic needs when dealing with product that needs to be
assembled either during development process or even after all of the design components
are complete. It is best that you follow all the sequences given and not to miss out any
notes provided in between the sequences.
Good luck…

Cast Iron Bracket - 125 -
CAST IRON BRACKET
First thing that we can see with this part is that it is symmetrical. So when starting to design
solid model, make sure that a datum plane is situated in the middle of the part. This datum
plane will help us align the component easily when doing assembly process. It should be
quite easy to develop solid model for this part.
Below is the available sequence for you to explore, but first always confirm that you are in
the correct working directory.
1. Create a new filename CAST_IRON_BRACKET. Uncheck the use default
mode.

- 126 - Cast Iron Bracket
4. Sketch a rectangle shown in figure 20-1 with all the dimensions given and
constraints indicated.
Please note that 76mm dimension comes from the addition of 50mm with both radiuses
R13mm from each side. Then we will protrude 10mm thickness for the rectangular block
which is the overall thickness of the bracket.
value to 10.0m > < enter>. Click to complete.
Set your view to Default Orientation, and your solid will look as shown in figure 20-2.
Next we will add a vertical wall which is 5mm offset from the Front plane. So we need to
create a new datum to make use of it as a new sketching plane.
6. Click icon and select Front datum plane to offset 5mm inside towards the
solid. Key in 5mm in the translation box from the Datum plane dialog box as shown
in figure 20-3.

Figure 20-3: Datum plane dialog box and the Offset plane.
7. With the new datum still highlighted, click > Sketch > and sketch a profile as
shown in figure 20-4 below.
Figure 20-4: Sketched profile.
Note that you need to add the centerline first before creating the profile. Both the additional
reference and the centerline are to assist your sketch by eliminating certain dimensions.
8. Then click icon to continue and update the depth value to 10.0mm and middle
click to complete.

Make sure that your solid creation is towards your previous solid. If not then, click icon
to toggle the direction of creation. The updated solid should look as shown in figure
20-5 below.
Figure 20-5: Updated solid profile.
9. Click icon > pick the two edges (figure 20-5) > update the round value to
16mm > to complete the sequence.
10. At Default Orientation, select the side wall surface (figure 20-5) > > Sketch
> Sketch > References > Add Additional References > Close > sketch two circles.
Figure 20-6: Constrained Circles.

11. Then click icon to exit from the sketching mode. Click on icon to create a
protrusion and update the depth value of 14mm from the dashboard. Use icon
to toggle the direction of creation. Finally click icon to complete the sequence.
12. Next, click icon > pick the two edges (figure 20-7) > update the round value to
13. At Default Orientation, select the Top Surface (figure 20-8) > > Sketch >
Sketch > References > Add Additional References > Close > sketch two circles
with diameter 13mm as shown in figure 20-9 below.

Figure 20-9: Two Circles with constrains.
cut and update the dashboard as shown in figure 20-10. Use icon to toggle the
direction of creation. Finally click icon to complete the sequence.
Figure 20-10: Updated dashboard requirement.
As you should know that we can actually do the holes by using the hole features itself. But
sometimes using the cut features may be more convenient here because you can make use
of the round edges of the plate created earlier as the main references for this hole creation.
Next is to create a right angle triangle rib at the middle of the bracket. Here we can do the
sketches using the Right Datum plane and protrude the solid evenly. So you need to
activate the Datum plane icon for this purpose.

15. At Default Orientation, select the Right Datum plane > > Sketch > Sketch >
References > Add Additional References > Close > sketch a right angle triangle
as shown in figure 20-11 below.
Figure 20-11: Sketched right angle triangle.
protrusion and update the depth value of 10mm from the dashboard. Use icon
to equally divide the direction of creation. Finally click icon to complete the
sequence.
Finally is to create a cut for a step design on to this bracket.
17. At Default Orientation, select the Right Datum plane > > Sketch > Sketch >
References > Add Additional References > Close > sketch a rectangle as shown in
figure 20-12 below.
Figure 20-12: Sketched rectangle for the step cut.

cut and update the dashboard as shown in figure 20-13. Finally click icon to
Figure 20-13: Updated dashboard.
Figure 20-14: Final Solid Creation.
Save your work.

Cast Iron Base - 133 -
CAST IRON BASE
We can see that this part is symmetrical on both sides, vertically and horizontally. So we
can make sure that two datum planes will equally divide the part and be the main
references during the assembly session. There are many ways to actually design this part
into solid and here is the shortest way of doing it.
First, always confirm that you are in the correct working directory.
1. Create a new filename CAST_IRON_BASE. Uncheck the use default template to
sketching mode.
4. Sketch the shape as shown in figure 21-1 with all the dimensions given and

- 134 - Cast Iron Base
Figure 21-1: Sketched part.
Please note that 66mm dimension comes from the subtraction of 146mm with both radiuses
R13mm and dimension 27mm from each side.
value to 76.0m and change the type of protruding into to equally distributing
the solid. Click to complete.
Next we will add rounds on all the four edges.
6. Click icon > pick the four edges (figure 21-3) > update the round value to

Cast Iron Base - 135 -
Figure 21-3: Rounded edges.
Finally is to add four holes to complete the design for this solid. Again we will use the
round edges as our references for the hole creation.
7. At Default Orientation, select the Top Surface (figure 21-3) > > Sketch >
Sketch > References > Add Additional References > Close > sketch four circles
with diameter 13mm as shown in figure 21-4 below.
Figure 21-4: Four Circles with constrains.
cut and update the dashboard as shown in figure 21-5. Use icon to toggle the
direction of creation. Finally click icon to complete the sequence.

- 136 - Cast Iron Base
Figure 21-6: Final Solid Creation.
Save your work.

Steel Shaft - 137 -
STEEL SHAFT
Revolve feature is the best method to produce this part. We may need to look at the
assembly method that we are going to apply when assembling this part onto the other
component of the Bell Roller. Since the shaft should be in the middle of the complete
assembly product, it is best to have a datum plane situated equally divided between the
solid created. Below is the sequence for creating solid of this component, but before
proceeding, always confirms your working directory.
1. Create a new filename STEEL_SHAFT. Uncheck the use default template to
3. Select the Right plane > > Sketch > to go onto the sketching mode.

- 138 - Steel Shaft
Figure 22-1: Sketched part.
5. Click icon to go back to 3D. Click icon > pick line X (see figure 22-1) >
to complete.
Next we will add smaller round solids on both end of the shaft using the same feature as
before.
6. Select the Right plane > > Sketch > Sketch > References > Add Additional
References > Close to go back to the sketching mode.

Steel Shaft - 139 -
7. Sketch two rectangles as shown in figure 22-3 with all the dimensions given and
Figure 22-3: Two rectangles added.
8. Click icon to go back to 3D. Click icon > pick line Y (see figure 22-3) >
to complete.
Figure 22-4: Updated Solid.

- 140 - Steel Shaft
9. Select the Surface (see figure 22-4) > > Sketch > Sketch > References > Add
Additional References > Close to go back to the sketching mode.
10. Sketch a circle as shown in figure 22-5 with all the dimensions given and
Figure 22-5: Circle sketched.
11. Click icon to go back to 3D. Click on icon to create a cut and update the
dashboard as shown in figure 22-6. Use icon to toggle the direction of
creation. Finally click icon to complete the sequence.
Finally is to add chamfer at both edge of the shaft.
12. Click icon and update the dashboard as shown in figure 22-7.

Steel Shaft - 141 -
Figure 22-7: Dashboard for chamfering.
13. Next pick the edge to be chamfered as shown in figure 22-8 and click icon to
complete.
Figure 22-8: Selected Edges
Finally your solid shaft should look like this:
Figure 22-9: Finalized solid.
Save your work.

- 142 - Steel Shaft
Notes:

Cast Steel Roller - 143 -
CAST STEEL ROLLER
This roller part can be design using revolve feature as well just like the shaft. May be the
tricky bit for this part is the sketch shape of the roller. The cross section is the shape that
needs to be drawn during the sketching mode. Below is the sequence for creating solid of
this component. Please make sure that your working directory is correct.
1. Create a new filename CAST_STEEL_ROLLER. Uncheck the use default

- 144 - Cast Steel Roller
Figure 23-1: Sketched section of Roller part.
5. Click icon to go back to 3D. Click icon > pick Centerline for Revolve
feature > to complete.
Save your work.

Bronze Bushing - 145 -
BRONZE BUSHING
Bronze Bushing is the simplest component of this assembly product and off course the
easiest way to design the solid is by using revolve feature. You may do your own self to
design this part, but here is one of the ways to create it. Please make sure that your
working directory is correct.
1. Create a new filename BRONZE_BUSHING. Uncheck the use default template to

- 146 - Bronze Bushing
Click icon to go back to 3D. Click icon > pick Revolve > to complete.
Save your work.

Bell Roller Assembly - 147 -
BELL ROLLER ASSEMBLY
First is that we need to know what are the parts to be assembled together and the parts must
be in the same folder with the assembly file. Also we need to be very careful with units’
correlation here. Different unit types can cause big problems into assembling any product.
Setting a proper unit when doing designing is very important and also the references of
each component plays major roles into developing an assembly product.
There are many ways to assemble this Bell Roller product. Which is the best way is the
question to be answered. First, we need to know which component of the assembly is the
fixed item. When assembled, no movement occurs on this component. This part would be
the best component to be as a default assembled part in the assembly. Here, we will
assemble the Cast Iron Base part first because it is a fixed component.
Please make sure that your working directory is correct.
1. Click icon and change the type from Part to Assembly and change the name
asm0001 to Bell_Roller. See figure 25-1 below.

- 148 - Bell Roller Assembly
Figure 25-1: New Dialog Box.
2. Uncheck Use default template to change the unit to mmns. Click OK to change the
unit as shown in figure 25-2 below.
Figure 25-2: Unit Dialog Box.

3. Then click OK to complete the sequence.
At this point, we have created an assembly file but no parts or components available inside.
So we need to assemble or bring them into this file. Proceed to the next sequence.
4. Click icon and choose Cast_Iron_Base.prt part file from the Open dialog box.
Click Open to continue.
5. From the dashboard expand the Automatic Assembly and click Default as shown in
figure 25-3.
Figure 25-3: Assembly dashboard.
6. Then select to complete the task.
Now you have added first component into the file and the position at default orientation is
as shown below in figure 25-4.
Figure 25-4: Cast Iron Base Plate added.

Note that if the position of your base is not the same as shown above, do not be worried.
This is because that when designing your base, you may have chosen different plane as
your sketching or possibly your second reference during selecting the sketching plane
might have oriented differently. For assembly purposes this should not be an issue as long
as you know which reference to choose to assemble the component.
Additionally, you also will notice that the Model Tree section has change with the base
assembled.
Figure 25-5: Model Tree for the assembly file.
Next is to add another component and this time is the Cast Iron Bracket part. We know that
this bracket has two holes with the same position and size with the Iron Base. We will use
these holes as our reference to assemble them together.
7. Click icon and choose Cast_Iron_Bracket.prt part file from the Open dialog
box. Click Open to continue and click to active the axis for assembly purpose.
Figure 25-6: Assembly References.

8. Select surface Side A > Side B (bottom surface of the bracket) as the first
reference.
Figure 25-7: First Reference selected.
Notice that the bracket is shifted upwards to level with the side A of the base and side B of
the bracket surfaces.
9. Next select the first axis combination which is axis A4 (see figure 25-6).
Figure 25-8: Second Reference selected.
Even though the status mentioned Fully Constrained, this component still can rotate about
the Axis A4 combination. So we need to add one more constrain to prevent this from
happening.

Figure 25-9: Assembly dashboard.
10. Click Placement > New Constraint > select the second axis combination which is
axis A3 (see figure 25-6).
11. Finally select to complete the task.
You updated assembly product should look like this:
Figure 25-10: Updated assembled product.
According to the assembly process for this product, two brackets are needed for this
assembly. We need to add the same bracket onto the other side of the base using the other
two axes A1 and A2 as part of the references.
Note that your assembly axes numbering might be different that from this module, but the
sequences of assembly should be similar.
12. Click icon > select Cast_Iron_Bracket.prt > Open.

Figure 25-11: Assembly References.
13. Select surface Side C > Side D (bottom surface of the bracket) as the first
reference.
14. Next select the first axis combination which is axis A1 and A3 (see figure 25-11).
Figure 25-12: Updated assembly process.

Notice that the new bracket is shifted to align with A1 and A3 together but facing
backwards. So we need additional reference to rotate the bracket and that is by adding
another axes combination of A2 and A4. (See figure 25-12)
15. Click Placement > New Constraint > select the second axis combination which is
axis A2 and A4 (see figure 25-11).
By adjusting the position of the present assembly product, your solid should look like this:
Figure 25-13: Updated assembled product.
17. Save your work. Click icon > <enter>.
It is a good practice to save your work even though it is yet to be completed. This is to
make sure that back up is there for you to retrieve if sudden issues occurred such as power
failure or your computer systems hang, and no recent data is available.
Next is to add or assemble the shaft. You can assemble different component such as the
roller if you know which reference to use. Here you will realize the benefit of pre-
arrangement of the datum plane in the component files.
18. Click icon > select Steel_Shaft.prt > Open.
19. Click to active the axis for assembly purpose unless it is already active during
the earlier session.

Figure 25-14: Axes reference.
20. Select the first axis combination which is axis A1 from the shaft and one of the
brackets (see figure 25-14).
At this point the shaft will move and aligned with the selected axes. You can actually move
the shaft by right clicking at the graphic area to pop-up a menu and select Move
Component.
21. Right-click at any graphic area > select Move Component > Left-click on the
shaft and move the cursor to adjust the position of the shaft to suit your needs (see
figure 25-15).
Figure 25-15: Pop-up menu.

When dealing with assembly files, you will need datum planes as references but not all are
required at a certain period of time. Also certain components which are already assembled
may not be relevant. So you need to hide it temporarily and you can do this when needed.
22. From the Model Tree, Right-click on the Cast-Iron-Base.prt > Hide to hide the
base part from the assembly.
23. Select icon > to deactivate datum axes and activate the datum planes.
Notice that the base part is not seen in the assembly. This will reduce the number of datum
planes activated and will ease the selection of datum planes needed for the next reference.
Continue with the next sequence.
Figure 25-16: Selected Datum Planes.
24. Click Placement > New Constraint > select Front Datum plane of the shaft and
ASM_Front Datum plane (see figure 25-16).
In the dashboard, make sure that the Align constrain is to make sure
that the shaft part is exactly in the middle of the assembly profile. Otherwise click
expansion mark and change it.
25. Finally select to complete the task. Click icon to close the datum planes.

Your updated assembly file is as shown below:
Figure 25-17: Updated Assembled product.
Remember that the Roller was designed with the datum planes created in the middle and
we know that this component is assembled in the middle of the shaft. So we do not have
any problems to hide both brackets in our assembly file as we did to the base earlier.
26. From the Model Tree, Press Ctrl Button > Pick on both Cast-Iron-Bracket.prt >
Right-click > Hide to hide the base part from the assembly.
27. Select > to activate the datum planes and axes.
28. Click icon > select Cast_Steel_Roller.prt > Open.
Figure 25-18: Selected Axes.

29. Next select the axis combination which is axis A1 from both the shaft and the roller
(see figure 25-18).
30. Right-click at any graphic area > select Move Component > Left-click on the
roller and move the cursor to adjust the position of the roller to suit your needs.
31. Click Placement > New Constraint > select Front Datum plane of the roller and
ASM_Front Datum plane.
32. Change the assembly constrain to > to complete the task.
Your updated assembly file is as shown below:
Figure 25-19: Updated Assembled product.
The last component to assemble is the bushing. This bushing is fixed to the center hole of
the roller and in between the shaft. So the main reference would be the axis of rotation for
both items and the mated surfaces between the bushing and the roller. The shaft can be
hidden too before the next assembly. Continue with the sequence.
33. From the Model Tree, Pick the Steel-Shaft.prt > Right-click > Hide to hide the
shaft part from the assembly.
34. Select to activate the datum axes unless it is already active.
35. Click icon > select Bronze_Bushing.prt > Open.
36. Select the axis combination which is axis A1 from both the bushing and the roller.
37. Next is to select surface A > surface B from the roller and the bushing respectively.
Figure 25-20: Selected surfaces.

38. From the dashboard, change icon to . This is to completely mate the two
surfaces.
39. Select to complete the task.
You can add another bushing with the same sequence but only on the other side of the
roller.
40. Click icon > select Bronze_Bushing.prt > Open.
41. Select the axis combination which is axis A1 from both the bushing and the roller.
42. Next is to select surface C > surface D from the roller and the bushing respectively.
Figure 25-21: Selected surfaces.
43. From the dashboard, change icon to . Change >
to complete the sequence.
After going thru this sequence, notice that every time we use axes as one of our assembly
reference, we only need minimum two references to complete the assembly requirement.
Also knowing the flexibility of hiding and unhide parts of the assembly will benefit the
user. Making use of the movement of parts during assembly sequence also helps the user to
rearrange the position for better and easier selection.
45. From the Model Tree, Press Ctrl Button > Pick all the hidden parts > Right-click
> Unhide to retrieve them back into the assembly view.
46. Save your work. Click icon > <enter>.

Your final assembly product should like this:
Figure 25-22: Final Assembly.
Notes:

APPENDIX B
ORTHOGONAL
PROJECTION
METAL PARTS

ii
FORKED BRACKET MILD STEEL SLOTTED LINK
FAN BRACKET MILD STEEL HALF CLIP

iii
CAST IRON FORKED END SHAFT BRACKET
SLIDING SUPPORT CAST IRON CRANK ARM

iv
GUIDE BRACKET V STOP
CAST IRON SUPPORT SIDE BRACKET

v
CAST IRON GUIDE BLOCK BRASS SUPPORT
CAST IRON JIG CAST IRON ROD GUIDE

vi
TRUSS BEARING
CAST IRON PULLEY GUIDE

vii
BELT-FORK BOSS
CAST IRON SUPPORT BRACKET

viii
CAST IRON BRACKET
CAST IRON END PLATE

ix
TAIL ROD GUIDE
CAST IRON PISTON

xi
RACK AND GEAR BRACKET
WORM GEAR BRACKET

xii
CAST IRON HOUSING
CAST IRON SUSPENSION BRACKET

xvi
PEDESTAL ROCKER ARM
SWIVEL BASE

APPENDIX C
ISOMETRIC
PROJECTION
METAL PARTS

ii
CAST STEEL WALL BRACKET CAST STEEL BRACKET
BRASS STEP CAST IRON BRACKET

iii
CAST IRON BENCH BLOCK MILD STEEL BRACKET
CAST IRON SUPPORT GRINDER REST

iv
JIG FRAME MILD STEEL ROD BRACKET
SAFETY BRACKET SUPPORT BRACKET

v
CAST IRON BRACKET CAST IRON SOCKET
MILD STEEL CLAMP MILD STEEL SLEEVE BRACKET

vi
CAST STEEL BRACKET CAST IRON JAW SUPPORT
OFFSET CRANK CAST IRON BEARING BRACKET

vii
BEARING RETAINER PUMP BRACKET
MAIN BEARING CAP

viii
BEARING PEDESTAL
CAST STEEL GUIDE BRACKET

ix
CAST STEEL JIG
SHAFT BRACKET

x
BEVEL GEAR SUPPORT
MILD STEEL CORNER SUPPORT

xi
CROSS SLIDE BRACKET
FLANGED SUPPORT OFFSET GUIDE

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