CO2 dragster car

Transcription

CO2 dragster car

CO2 dragster
Pro|ENGINEER - Wildfire 3.0
CO2 dragster
Schools and Schools Advanced Edition
.3-0002
W3-SE-L1-006-1.3
Pro|ENGINEER Wildfire 3
CO2 dragster
Written by Tim Brotherhood These materials are © 2007, Parametric Technology
Corporation (PTC)
All rights reserved under copyright laws of the United
Kingdom, United States and other countries.
PTC, the PTC Logo, Pro|ENGINEER, Pro|DESKTOP,
Wildfire, Windchill, and all PTC product names and
logos are trademarks or registered trademarks of PTC
and/or its subsidiaries in the United States and in
other countries.
Conditions of use Copying and use of these materials is authorised only
in the schools colleges and universities of teachers
who are authorised to teach Pro|ENGINEER in the
classroom.
All other use is prohibited unless written permission is
obtained from the copyright holder.
Acknowledgements Gavin Quinlan – Honeycomb Solutions
Proofing and comments – Andrew Dissington
Trialing materials – Schools attending INSET in
Ireland at Honeycomb Solutions - Autumn 2006
Feedback In order to ensure these materials are of the highest
quality, users are asked to report errors to the author.
Suggestions for improvements and other activities
[email protected] would also be very welcome.
Product code W3-SE-L1-006-1.3
http://www.ptc.com/company/community/education/
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Contents
CO2 dragster............................................................................................................ 1
Pro|ENGINEER - Wildfire 3.0 Schools and Schools Advanced Edition ....................... 1
Contents................................................................................................................... 3
Introduction........................................................................................................... 5
Abbreviations and terminology............................................................................... 5
Background.............................................................................................................. 6
Project briefing ......................................................................................................... 6
Lesson one – Competition rules................................................................................... 7
Lesson two – Model car body..................................................................................... 8
Shaping strategies ................................................................................................. 8
Task one – Getting started ...................................................................................... 9
Task two - Side profile ......................................................................................... 12
Task three - Plan shape ........................................................................................ 18
Task four - Rounding corners ................................................................................ 23
Task five - Adding material .................................................................................. 24
What you have learned in session two .................................................................. 29
Lesson three – CNC Machining ................................................................................ 30
Lesson four – Part properties and own design ............................................................ 32
Task one - Component information ....................................................................... 33
Task two - Changing the appearance .................................................................... 34
Task three - Measure mass of body ....................................................................... 36
Task four - Modify body shape ............................................................................. 38
Failed features..................................................................................................... 40
What have you learned?...................................................................................... 45
Session five – Assembly ........................................................................................... 46
Task one - New assembly with fixed car body........................................................ 47
Task two - Assemble rear axle .............................................................................. 49
Task three – Assemble front axle ........................................................................... 51
Task four – Kinematic movement........................................................................... 52
What have you learned ....................................................................................... 53
Lesson six – Surface finishing own design ................................................................. 53
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Lesson seven – Testing own design ........................................................................... 54
Lesson eight – Refine own design ............................................................................. 55
Lesson nine – Finish own design + Technical drawing ................................................ 56
Task one - Creating a drawing ............................................................................. 57
Task two - Adding dimensions .............................................................................. 62
Task three – Pictorial view .................................................................................... 66
Task four - Adding notes ...................................................................................... 68
What have you learned ....................................................................................... 71
Lesson ten – Rendered image ................................................................................... 71
Task one - Getting started .................................................................................... 72
Task two - Initial render settings ............................................................................ 74
Task three - Load scene ........................................................................................ 75
Task four - Position model in room ........................................................................ 76
Task five - Change view of model ......................................................................... 78
Task six - Render ................................................................................................. 79
Task seven - Save rendered image ........................................................................ 81
What have you learned this session? ..................................................................... 81
Lesson eleven – Testing modified design.................................................................... 82
Lesson twelve – Presentations ................................................................................... 83
Module review........................................................................................................ 83
Extension activities............................................................................................... 84
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Introduction
This CO2 dragster project introduces you to the skills and techniques needed to visualise
design ideas using Pro|ENGINEER Wildfire 3.0.
During these tutorials you will learn how to create parts, assemblies, rendered images
and technical drawings using Pro|ENGINEER Wildfire 3.0 and working as a team.
This tutorial and teacher resource has been produced by PTC© in support of the PTC
‘Design & Technology in Schools’ programme.
Abbreviations and terminology
Left-click
Left-click-drag
Press and release the left-hand mouse button
Press and hold-down the left-hand mouse button and move the
mouse
Right-click
Press and release the right-hand mouse button
Right-hold
Press and hold-down the right mouse button
Middle-click
Middle-click-drag
Press and release the middle mouse button
Press and hold-down the middle mouse button and move the
mouse
Sample files
You will need sample files to carry out this activity. Your teacher will show you how to
copy these into your working area.
Axle.prt
(Pro_standards) A3_FORMAT.frm
BALSA.jpg
Balsa_wood.mat
Car_assy.asm.1
Car_04.asm.1
Car_assy_sim.asm.2
Extrude_04.prt.1
Body_01.prt
Front_axle_assy.asm.2
Body_extrude.prt
Rear_axle_assy.asm.2
Body_extrude_02.prt
Wheel_front.prt.3
Body_extrude_sim.prt
Wheel_front_sim.prt.3
Bright_white.scn
Wheel_rear.prt.3
Car_03.asm.1
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Wheel_rear_sim.prt.1
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Background
Racing CO2 powered cars originated many
years ago in the US and competitions have
now spread to most parts of the world.
There are a many web sites with information,
examples and advice on the design,
construction and testing of the cars.
However, when designing your car, make sure
you comply with the rules for your region.
Project briefing
These materials will show you how to use
Pro|ENGINEER to create a Parametric 3D
model of your car design, create a rendered
image and engineering drawing.
Standard components such as wheels and axles
are provided
When machined on a CNC router, finished by
hand and assembled the models should be
ready to race!
‘Start your engines’ and good luck!
Module - Learning objectives
By the end of the module you should:
Be aware:
•
of the concepts of 3D parametric solid modelling using Pro|ENGINEER
•
of aerodynamic testing using Computational Fluid Dynamics (CFD) software.
Understand:
•
the principles of 3D parametric solid modelling using Pro|ENGINEER
•
how 3D solid modelling software be used to refine designs including parts and
assemblies.
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CO2 dragster
how CFD software simulates aerodynamics and can help with body design.
Be able to:
•
create 3D solid model components from scratch using extrusions with internal
sketches and rounds
•
assemble components using assembly constraints
•
carry out CFD analysis on their car design. Note: this requires Pro|ENGINEER
Schools Advanced Edition and additional software.
Lesson one – Competition rules
Aim:
You will be able to familiarise yourselves with the challenge and competition rules and
begin to suggest designs for the car.
Objectives:
By the end of the session you should be:
Aware of
•
the overall goal in the competition.
•
the competition rules and the implications of not adhering to them
•
the factors that impact on car performance.
Understand
•
the technical detail contained in the rules and how these relate to car performance.
•
the scientific principles that govern how fast cars travel
Be able to
•
apply the competition rules to car design.
•
suggest car designs that comply with the rules and optimise car performance.
Focus:
During this session you will have the opportunity to develop an understanding of the
competition rules and the scientific principles that govern car performance. This may be
through lecture, experimentation or simulation.
You should be able to analyse existing designs for compliance with rules and predict how
efficient the design is. With this knowledge and understanding you should be able to
suggest design variations that comply with the rules and might improve the performance
of the car.
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This session is now complete.
Lesson two – Model car body
Aim:
You will be taught how to use Pro|ENGINEER parametric 3D modelling software to
create a car body component for the CO2 car competition.
Objectives:
By the end of this session you should:
Be aware of
•
the concepts of 3D parametric modelling.
•
the modelling capabilities of Pro|ENGINEER.
Understand
•
how 3D modelling software can help designers and engineers try out ideas and
refine the detailed design of products.
•
the procedures involved in modifying Pro|ENGINEER models.
•
the importance of Parent/child relations in parametric modelling.
Be able to
•
create extrude features and rounds to modify an existing Pro|ENGINEER
component.
Focus:
In this session you are taught how to use Pro|ENGINEER to modify a 3D parametric
model of a balsa blank to create a car body design using extrude and round features.
Shaping strategies
There are several methods you could use to
shape the body of your car.
This tutorial provides a part that represents
the balsa blank
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You will be shown how to remove material
from the part to get the shape you want.
You could also create the shape from
scratch by adding material.
Each of these methods, removal or addition of material, can be done using a number of
different Pro|ENGINEER software tools.
For simplicity and to build on schools experience with Pro/DESKTOP, you will be shown
how to use extrusions, rounds and holes.
Task one – Getting started
1. Start the Pro|ENGINEER program.
The Pro|ENGINEER screen
As you work through this tutorial you will soon become familiar with the Pro|ENGINEER
screen, menus, dashboard and dialog windows.
It is worth having the Pro|ENGINEER Quick Reference Card available as a reminder of
the key functions, toolbars and techniques. This can be downloaded from the default
home page displayed in the browser of Pro|ENGINEER.
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Note: In Pro|DESKTOP the left panel is usually referred to as the ‘Browser’ window.
Pro|ENGINEER uses this term for the embedded web browser. For this reason the left
panel in Pro|ENGINEER is called the ‘Navigator’ window. It can present several
different views
Folder Navigator
Model tree Navigator
The other two tabs will not be used in this tutorial.
Tip:
Don’t be tempted to maximise the Pro|ENGINEER window. There should be a
gap down the right hand side of the window where dialogs will appear.
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Set working directory
2. The Navigator window on the left of
the screen should be displaying
folders.
3. Browse to the folder you will be saving
your work and where the sample files
have been saved.
Your teacher will tell you where this is.
4. Right click over the folder and from the
floating menu select Set Working
Directory.
5. In the Navigator window select the folder where the sample files are stored for this
tutorial.
The browser window will display a list of files.
6. Locate and click on the file named
BODY_01.PRT
The model will preview in the top of the
browser window
7. Click on
, the Open File… button.
The browser window will close and the
balsa block part will appear in the graphics
window.
On your screen you may see a clutter of
brown lines.
These are datum planes and axes and the
display of these can be toggled on/off.
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8. In main toolbar across the top of the
screen, find the datum view tools then
click on each one until the model is
clearly visible.
Parent child relationships
Look at the model tree in the Navigator
window. Each entry represents an element
of the model
•
Part
•
Datum planes
•
Coordinate system
•
Sketch based feature
•
Internal sketch
•
Direct feature
The concept of parent/child relationships is fundamental to Pro|ENGINEER. Almost
every action relies on previous actions. This may be drawing geometry, features or
components. A good example is the hole above. The hole was placed on the rear surface
of the block and relies on this face existing.
If the extrude feature that created the face is deleted the round will also be deleted.
The model display lists datum planes, features, parts, etc in the order they were created.
In a moment you will add features to the model and they will appear in the model tree.
Task two - Side profile
For simplicity you will shape the side profile of the car. This requires an extrude feature
removing material.
1. In the toolbar on the right of the screen select
, the Extrude tool.
The extrude ‘Dashboard’ will appear along the bottom of the screen.
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This is a very clever way of presenting a number of options that would require several
dialog windows.
Underneath the extrude dashboard you should see a line of text with a green arrow next
to it. This is the prompt line and is visible all the time.
It is very important you keep an eye on the prompt area. Here Pro|ENGINEER tells you
what it is doing or what it expects you to do next. At the moment it is asking you to select
or define a sketch. You will do the second of these.
Defining a sketch
2. In the main toolbar across the top
of the screen, click on
, to make
datum planes visible in the model.
This tool toggles, so keep clicking until
you can see the brown lines and text
shown here.
The profile will be sketched on the
FRONT datum plane running
lengthways through the block.
3. In the dashboard click on the word
Placement to open a pop-up panel.
4. Click on the
.
The Sketch dialog opens in the top right
corner of the screen and the prompt
area at the bottom of the screen is
asking you to ‘Select a plane of surface
to define the sketch plane’.
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5. Move the mouse cursor over the
model and as you do this different
parts of the model or workplanes
will change colour to cyan (light
blue). This is called prehighlighting.
6. When the FRONT datum plane is
pre-highlighted cyan, click to select
it.
The datum plane will change colour to
orange to show it is selected.
Look at the Sketch dialog. The
word FRONT appears in the
Sketch Plane field and other
options have been filled in for you
by Pro|ENGINEER.
7. Accept the defaults and click
on
.
A number of things will happen.
The sketch dialog will close and
the model will rotate until the front
datum plane is parallel to the
screen.
The dashboard will be paused
(greyed out) and a sketcher
toolbar will replace the feature
creation toolbar on the right of
the screen.
8. In the main toolbar click on
to change view to Hidden line.
coordinate systems.
and
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to turn off the display of datum planes and
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Creating references
To use best practice when modelling, sketched lines should be constrained to existing
solids and geometry. To achieve this we will need a reference line along the front face of
the balsa block.
10. Open the Sketch pull-down menu and
select References.
The References dialog will open
11. In the graphics window select the vertical
front edge of the balsa block.
A dashed brown vertical reference line will
appear at the front of the block and an extra
entry will be added to the References dialog.
12. Click
.
You are now ready to sketch
the shape to be removed
from the balsa block.
The hole for the CO2 canister should be clearly visible. The cut you will sketch must be
above this hole.
Sketching lines
13. In the sketcher toolbar on the
right of the screen, select
the Line draw tool.
14. Left click at each of the
locations on the green line X1 –
X3
X1
X2
X3
the
15. Middle mouse click twice. The
first to stop drawing joined lines
and the second to cancel the
line draw tool.
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The lines may need moving to clear
the CO2 cartridge hole and/or
prevent the nose becoming too thin.
16. In the sketcher toolbar on the
right of the screen, make sure
the Select Items tool is
active.
17. Click on the horizontal line for
the nose then release the mouse
button.
The line colour will change to red to
show it has been selected.
18. Move the mouse cursor over the
selected line, click and hold the
left mouse button and drag the
line upwards until the
dimension is just less than 20
mm.
Later you will learn how to alter the dimensions directly to control the shape and position
of sketch lines.
These three connected lines will be used to slice the top off the balsa block.
19. In the sketcher toolbar on the right of the screen click on
to close sketcher.
to change the view to Shading.
Isometric.
, the saved views list and select Trimetric or
Completing the extrusion
The extrude dashboard was greyed out while you were in sketcher. It should now be
active along the bottom of the screen.
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In the graphics window you will be
able to see a preview showing the
cutting surface coloured green based
on the line you drew. The yellow
arrows show the direction of the
extrude and the side material will be
removed from.
22. If necessary, click on the yellow
arrows to make them point in the
directions shown here.
Currently the extrude operates in only
one direction.
23. In the dashboard click on the
buttton.
A pop-up panel will open.
24. Change the settings to those
shown here.
25. In the dashboard, the option to remove
material
should be selected.
26. No more changes are needed so click
, at the right of the dashboard to
on
complete the extrude.
The top surface of the block will now be
stepped.
27. Save your model.
The next step will use the same technique to shape the sides of the car by extruding a
sketch upwards.
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Task three - Plan shape
1. Make sure datum planes are visible in the
model.
2. In the feature creation toolbar click
,
Extrusion. The extrusion dashboard will
open along the bottom of the screen.
The profile will be sketched on the TOP datum
plane running along the base of the block.
Last time you opened the Placement slide up
panel to select the sketch plane. This time you
will use an alternative method.
3. In a blank area of the graphics screen
click and hold the Right mouse button.
4. From the floating menu select Define
Internal Sketch…
5. In the graphics window click to select the
TOP datum plane.
Pro|ENGINEER will populate the other options
in the Sketch dialog.
6. Click on
dialog.
, to close the Sketch
The sketcher toolbar will appear on the right of the screen, the dashboard will be greyed
out and the model will rotate to view the sketching plane perpendicular to the screen.
Here you are looking down on the balsa block.
The sketch you will create will look like the green line in the next illustration.
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Drawing a centre line
Later in this section we will need to mirror a set of lines. In order to do this a Centerline
(sic) is required so this will be created first.
7. In the sketcher toolbar click on the small triangle next to
8. In the fly-out menu select
, the Line tool.
, the Center line tool.
9. Move the mouse over the dashed orange reference line running down the centre of
.
the model. You will see a coincident geometric constraint symbol.
10. When you see this symbol click to locate one point for the centre line.
Move the mouse along the dashed reference line and you will see a pair of red lines
showing the centre line will be co-linear with the reference line.
11. When you see this symbol click to locate another point and complete drawing the
centre line.
Drawing the nose circle
12. In the sketcher toolbar select
, the Circle draw tool.
13. Move the mouse over the centre line.
Look for the coincident constraint feedback at the cursor position.
14. Click at the X1 to locate the centre of the nose circle.
X2
X1
15. Move the mouse a small distance and you will see a rubber band circle. Click at the
second position X2 to complete drawing the circle.
16. The circle tool is still active. We don’t want to draw any more circles so:
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17. Click with the middle mouse button to finish drawing circles.
Notice Pro|ENGINEER has created dimensional constraints coloured grey for the distance
of the circle from the vertical reference line and for the diameter of the circle.
The grey colour denotes ‘weak’ dimensions. You will change the value of these and
Pro|ENGINEER will automatically make them strong and locked. Later in this tutorial
there is an explanation of the different types of dimensional constraint.
18. Double click on the horizontal
dimensional constraint.
19. The value will become editable
20. Type in 250 for the value and hit Enter
on the keyboard.
The circle will move along the centre line until the centre is 250mm from the vertical
dashed line. Notice the dimension is now orange showing it is a ‘strong’ dimension and
locked.
21. Double click on the circle diameter
constraint.
22. Change the value to 15 mm and hit
Enter on the keyboard.
The diameter dimensional constraint has
turned orange showing it is now a strong
and locked measurement.
Remember how we made the cartridge hole visible?
23. In the main toolbar, click on
24. In the sketcher toolbar activate
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, to change the view to wire frame.
, the line draw tool.
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25. Draw the lines shown here by clicking at each of the positions shown (X1-X3). Before
clicking at position X3 make sure you can see a ‘T’ symbol to denote you will be
creating a tangent geometric constraint.
X1
X2
X3
26. Middle mouse click to finish drawing connected lines and middle mouse click again
to cancel the line draw tool.
This shape will now be mirrored to create a symmetrical body shape.
Mirror geometry
27. In the sketcher toolbar make sure
, the Select tool is active.
28. Click on one of the lines you have just drawn to select it. It will turn red.
To add lines to the selection you will need to use the CTRL key on the keyboard.
29. Hold down the CTRL key and click on each of the lines in turn until both are selected
like this.
30. In the sketcher toolbar click on
, the Mirror tool.
In the prompt area at the bottom of the screen Pro|ENGINEER is asking you to ‘Select a
Centerline’.
31. Click on the horizontal centre line running through the middle of the sketch.
The selected lines will be mirrored.
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Notice the blue arrows pointing to the centre line. These indicate mirror constraints.
One thing remains to be done, parts of the nose circle need to be trimmed.
Trimming lines
You have used the trim tool already. This
time you will use it in a slightly different
way.
32. Use the middle mouse wheel to zoom
in tightly over the nose circle.
Trim tool.
, the
X2
34. Click and hold the left mouse button at
position X1 then drag to draw the line
to position X2.
X1
35. The plan sketch is now complete.
close the sketch.
, to
37. The dashboard is now active.
change the view to Shaded.
, to
, the
saved views list and select Trimetric or
Isometric.
40. You will be able to see a preview
showing material will be added to one
side of the sketch by a random value.
41. Notice the yellow arrows. The vertical
arrow show the direction of the extude
and the horizontal arrow shows the
side of the line the extrude will be
applied.
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42. In the graphics window click on the
horizontal yellow arrow to change the
side of the line the extrude will act on.
43. In the dashboard change the Extrude
direction to
‘Intersect with all
surfaces’.
44. Make sure
, is selected (remove
material) in the dashboard .
45. No more changes are needed so click
on
, at the right of the dashboard to
complete the extrude.
46. Your car body should now look like
this.
Task four - Rounding corners
The next step is to round the corners to make the shape more aerodynamic. Rounds are
called ‘Direct’ features because they do not require sketches. They do however rely on
existing 3D geometry as a ‘Parent’ and are ‘Children’ to it.
Remember if the ‘Parent’ solid geometry disappears the ‘Child’ feature will also
disappear.
1. In the sketcher toolbar select
Round tool.
, the
X1
2. In the graphics window select the edge
labelled X1.
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3. Hold down the CTRL key and select the
other edges shown here in red.
Notice some edges select automatically.
Look at the geometry of these lines and try
to suggest a reason for this?
4. To change the radius to 5 mm either
drag the radius handle or alter the
value in the dashboard.
5. Click
, the green tick in the
dashboard to complete the round.
The car body should now look like this.
Tangential edges
The reason some edges
selected themselves was
because they were tangential
to one that was selected.
T
Tangents between edges exist
at the points arrowed with a
red ‘T’
T
Task five - Adding material
So far we have removed material from the
block. We now want to create a wing fairing
to streamline the airflow around the front axle.
You will start an extrude, create an internal
sketch on the front datum plane and then
complete the extrude, symmetrical about the
datum plane.
1. Make sure datum planes are set to be
visible.
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2. In the feature creation toolbar click
the Extrude tool.
,
3. In a blank area of the graphics window
click and hold the left mouse button.
4. From the floating menu, select Define
Internal Sketch...
5. In the graphics window click to select the
FRONT datum plane.
6. Click on
dialog.
, to close the sketch
7. The model will rotate on screen until the
sketch plane is parallel to the screen.
8. Zoom in to the nose of the car body.
9. Draw a circle half way up the nose of the
car.
10. Alter the dimensional constraints to the
values shown.
Construction lines
First you will create construction lines to help draw the aerofoil shape. To make sure the
aerofoil remains symmetric the construction lines will be created with an ‘equal length’
constraint.
11. In a blank area of the graphics screen
hold down the right mouse button.
12. From the floating menu select
Line.
13. Click at the centre of the circle you have
just drawn.
14. Move the mouse to the left and when you
see the H, horizontal constraint click to
draw a horizontal line.
X1
X2
15. Middle mouse click to finish drawing
joined lines.
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16. Click in the centre of the circle X1.
17. Move the mouse to the right and wait until
you see a ‘H’ horizontal constraint and L1
equal length constraints before you click
X2 to draw the line.
X1
X2
18. Middle mouse click twice, once to finish
drawing joined lines and a second time to
cancel the line draw tool.
Converting lines to construction
19. Click on one of the lines you have just
drawn to select it.
20. Hold down CTRL on the keyboard and
click on the other line.
21. Click and hold the right mouse button and
from the floating menu select
Construction.
22. Change the horizontal line dimension to
25 mm.
X2
23. Draw the line shown X1- X2 making sure
there is a tangent ‘T’ constraint when you
click at X2
X1
24. Middle mouse click to stop drawing
joined lines.
25. Draw three other lines from the ends of
the horizontal lines to the circle.
Tip: don’t forget to middle mouse click once
after each X2 click to stop drawing joined
lines.
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X2
X1
X1
X2
X2
X1
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Trimming lines
Remember the two methods of trimming line segments? You can click on a segment to
delete it or hold down the left mouse button and ‘scribble’ across several lines to erase
them.
26. Use
the Trim tool to erase parts of the
circle to leave the shape shown here.
finish sketching.
change the view to Shaded.
, to
, to
, the saved
views list and select Trimetric or Isometric.
30. You will be able to see a preview showing
material will be added to one side of the
sketch by a random value.
The dashboard will become active.
31. In the dashboard, change the extrude
direction to symmetrical
.
32. Change the extrude distance to 35 mm
(minimum body width at the wheels in
the rules).
33. Click
, to finish the Extrude feature.
Task five - Adding rounds
You will now add rounds to the join between the wing and body. This is for two reasons;
to smooth the airflow and to reflect the limitations of using a ball nosed cutter when
machining the body.
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1. In the feature creation toolbar click on
, the Round tool.
2. Holding down the CTRL key on the
keyboard, click to select the leading
and trailing edges of the wing on both
sides of the nose.
3. In the dashboard set the radius to 0.5
mm.
4. Click on
to complete the round.
5. In the feature creation toolbar click on
, the round tool.
6. Holding down the CTRL key on the
keyboard, click on edges where the
wing joins the nose.
7. Change the radius to 5 mm.
8. Click on
to complete the round.
Task six - Axle holes
Pro|ENGINEER has a dedicated tool that we will use to create the axle holes for the
axles.
1.
In the feature creation toolbar click
, the Hole tool.
2. Select the side of the wing as the
surface the hole will be placed on.
X1
X2
X3
A dashboard will open and the hole will
preview.
There are three handles on the preview;
one for the depth X1 and two for the
placement X2, X3.
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3. Drag one of the placement handles to
the rear surface of the body. Release
the mouse button when the rear face is
highlighted.
4. Drag the other placement handle onto
the base surface of the body. Release
the mouse button when the bottom face
is highlighted.
5. Alter the placement constraints to 220
mm and 10 mm as shown.
6. In the dashboard, change the depth
option to
‘Drill to intersect with all
surfaces’.
7. Click
to complete the hole
definition.
8. Add another hole for the rear axle
using the values shown here.
To complete the body we will change the material to balsa and apply a texture to the
surface.
What you have learned in session two
Objectives:
Having completed this session you should now:
Be aware of
•
the concepts of 3D parametric modelling.
•
the modelling capabilities of Pro|ENGINEER.
Understand
•
how 3D modelling software can help designers and engineers try out ideas and
refine the detailed design of products.
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•
the procedures involved in modifying Pro|ENGINEER models.
•
the importance of Parent/child relations in parametric modelling.
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Be able to
•
create extrude features and rounds to modify an existing Pro|ENGINEER
component.
Lesson three – CNC Machining
Aim:
During this session you will be shown how a car body design is post processed and
machined using a CNC router. You should gain sufficient awareness of machining to
help you design car bodies within the limitation of machining.
Objectives:
Be aware of
•
the capabilities of three axis CNC machines.
Understand
•
how post-processor software interprets the 3D model and produces movement
instructions to steer the cutting tool.
•
how jigs and fixtures can reduce the setup time for machining identical parts.
•
and implement health and safety control measure when working with CNC
machines.
•
the limitations of 3 axis CNC machining and how this influences designs.
Be able
•
under close supervision, to setup up and carry out the machining of their car body
design.
•
to suggest designs it is possible to machine.
Focus:
It would be very easy for you to come up with car body designs that cannot be machined.
This session demonstrates the post processing and machining sequence during which your
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teacher will explain limitations such as tool diameter/tip shape, avoiding undercuts and
hollows.
Where possible you should be able to use CNC equipment at school or locally to machine
your car design. If this is not possible machining may need to be done elsewhere.
Where remote manufacture is the only option investigate whether web camera viewing of
the machining is possible.
Because post processor and CNC software is specific to each manufacture it is not
possible to write a detailed tutorial however the principles involved are explained in the
following diagram.
Post
processing
Machining
Machine
instructions
Pro/ENGINEER
model
3 axis CNC
machine
Machining a CO2 car body
and finished car
CNC machining and Car images - Lochgelly High School, Scotland
www.detinschools.co.uk
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Lesson four – Part properties and own design
Aim:
Learn how to use Pro|ENGINEER to measure the properties of a part and modify the car
body design.
Objectives:
Be aware
•
that properties can be applied to components and used to make measurements.
•
that Pro|ENGINEER can calculate physical properties of components.
•
that Pro|ENGINEER allows the user to modify parts very easily.
Understand
•
how critical dimensions and geometry in parametric 3D models can be used to
modify the design.
•
the opportunities provided in Pro|ENGINEER for physical analysis of models
and assemblies.
Be able to:
•
assign component information including material properties to a model.
•
change a design by altering dimensions and geometry.
•
Be able to apply material properties to parts
•
Be able to use Pro|ENGINEER to take simple measurements from components.
•
Be able to make change to their design prompted by analysis and
measurements.
Focus:
One of the key benefits of parametric modelling is the facility Pro|ENGINEER has to
change designs very quickly and report the physical properties of parts.
To realise the full power of parametric models they need to be created with future
modifications in mind.
This section teaches you how to use Pro|ENGINEER to report physical properties for a
part and edit an existing model to alter the design.
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Task one - Component information
It is good practice to add information to components. This helps trace parts and will also
populate part tables in drawings automatically.
Set material properties
When you create parts it is important to set the correct material so that subsequent
analysis accurately represents the component behaviour. Pro|ENGINEER has a
comprehensive materials library.
1. Your car body should be open on screen.
2. From the Edit pull-down text menu select Setup
Menu manager will open at the
right side of the screen.
3. Select Material.
The Materials dialog will open.
4. Browse to the folder where
material definitions are
stored and select
balsa_wood.mat
5. Click on
to transfer the
material to the Materials in
Model column.
6. Click on
to close
the Materials dialog.
7. In Menu Manager click on
Done to close it.
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Component parameters
8. Your car body should be open on screen.
9. In the Tools pull-down text menu select
Parameters…
The Parameters dialog opens.
Notice the material balsa you selected a moment
ago has already been entered for you.
10. In the left column select DESCRIPTION then click
on
.
The Parameter Properties dialog opens.
11. Type your name in the Value field then click
.
12. Use the same technique to complete the
MODELLED_BY and PROJECT fields.
13. Click on
dialog.
to close the Parameters
14. Save your model.
Task two - Changing the appearance
Pro|ENGINEER is provided with a great many
material textures that can be applied to your
models. Balsa wood is not one of them so you will
be shown how to create a new texture and then
apply it to your model.
1. Open the View pull-down text menu.
2. Select Color and Appearance.
The Appearance Editor will open.
3. Click on the + sign to create a new entry based
on the default material.
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4. In the space below the material thumbnails,
type a name for the material then press Enter
on the keyboard.
5. Half way down the Appearance Editor dialog,
click on the Map tab.
6. You will add a bitmap image in the Color
Texture option.
7. Click on the large button in the Color Texture
section of the dialog (shown here by the red
rectangle).
The Appearance Placement dialog will open.
8. Open the File pull down menu and select
Open.
9. Browse to the location of the BALSA.jpg file,
select it then click on
.
BALSA.jpg will now be listed in the Appearance
Placement dialog.
10. Click on the new entry for balsa to select it.
11. Click on
to finish with the Appearance
Placement dialog.
The Appearance Editor should still be open on
screen.
Notice there is a new entry for balsa in the
thumbnails and the ball looks like balsa.
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Saving the list of materials
12. Open the File menu and click on Save.
13. Type a name for the new list of materials
then click on
dialog.
to close the Save
14. In the Appearance Editor click on
to transfer the balsa texture onto the car
body model.
15. Click on
to finish with the
Appearance Editor.
The model now has the appearance of balsa.
Task three - Measure mass of body
Working out the volume and mass of a regular geometric shape is not too difficult.
length x width x height
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Π x radius2 x height
Π x radius2 x height/2
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With complex shapes it is much more difficult working out
the volume and without physically making your model it
would be very difficult to find out the mass.
Pro|ENGINEER has tools that can measure all the
physical properties of the model. This includes density
and mass because you have allocated the material
properties of balsa to your model. We can now ask
Pro|ENGINEER to work things out for us.
1. At the top of the screen open the Analysis pull-down
menu and click on Model.
2. In the fly-out menu select Mass Properties.
The Mass Properties dialog will open.
3. Click on
the Compute… button
in the left corner.
The dialog will show details for the
model. This includes many properties we
are not concerned with.
We are interested in the MASS entry
which works out at 37.33 grams.
This is well below the minimum weight of
55 grams but doesn’t allow for the
weight of filler and paint.
Before closing the dialog, find the CENTER OF
GRAVITY entry and notice the x, y and z
coordinates. Now look in the graphics window
(you may need to drag the dialog to one side).
There two sets of axes in the model. Reference
axes at the bottom rear of the body and axes in
the middle of the body at the centre of gravity.
The x, y and z values in the dialog are
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distances between these two sets of axes.
Design considerations
As you develop your design you can carry out repeated analyses to check it complies with
regulations. You may decide to measure the exact density of the balsa block you will be
using as it can vary quite a lot.
If you could choose between a dense block of balsa and a less dense one, which would
you go for? To help you, all other things being equal, it is best to keep the frontal area to
a minimum.
Task four - Modify body shape
1. Your car body model should be open
in Pro|ENGINEER with your part
folder set as the working directory.
The body should look like this
The navigator panel on the left of the
screen will be showing the model tree.
In this example the Extrude 1 entry has
been expanded to show the internal
sketches.
2. In the model tree, left click on the
internal sketch for Extrude 1.
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In the graphics window the sketch lines
will be visible and highlighted in red.
The surfaces created by extruding the
sketch lines may also be highlighted.
To change the body shape, the sketch will
need to be edited.
3. In the model tree, move the mouse
cursor over the internal sketch for
Extrude 2 and right mouse click.
4. From the floating menu select Edit
Definition.
Entries in the model tree below the sketch
will be hidden, the selected sketch will be
opened, the sketcher toolbar will appear
and the graphics window will display the
sketch lines.
You may have decided to lengthen the
horizontal line over the CO2 hole.
5. Double click on the dimension
constraint and alter it to 70 mm.
Notice the dimension has changed to
orange. This will be explained later.
What if we wanted to shorten the nose to
30 mm? There is no dimension to do this.
X1
Create defining dimension.
7. Left click on the green line at X1 to
select the line then middle click at X2
to locate the constraint text.
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X2
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8. Double click on the new dimension
constraint and change it to 40 mm.
9. In the sketcher toolbar, click on
close the sketcher.
to
The model should regenerate and display
the new shape.
There are occasions when features lower
down the model tree cannot be
regenerated due to the changes you have
made.
The following guide may be useful if you
get an error at this stage.
Failed features
These are typical error dialogs when regeneration fails.
The Failure Diagnostics window explains in detail what has failed and why.
In this example the #9 feature in the model tree, a ROUND on the component called
BODY_10, failed because Feature references are missing.
This is a perfect example of the importance of parent/child relationships. Some of the
reference edges in the ‘parent’ solid are missing for the ‘child’ round to regenerate.
We can deduce from this information that changes we have just made to the car body
profile have removed edges the rounds relied on.
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The original shape.
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Can you spot the missing edge
references in the round set on the left?
The Menu manager on the right of the screen provides a number of
options for resolving the problem.
Undo changes – Roll-back the changes you just made to a state the model tree could be
regenerated.
Investigate –
Find out more about the failure.
Fix model –
Access the model tree and make changes to resolve the failure.
Quick fix –
The most common starting point for fixing the problem and the one we
will demonstrate here.
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10. In the Menu Manager click on Quick fix.
The Quick fix menu opens on top.
11. Select Redefine.
A Confirmation menu is added on.
12. Click on Confirm.
The Round dashboard
will appear along the
bottom of the screen and
the model will try to
preview round edges.
Because the round failed
the round will not
preview.
13. In the dashboard, open the Sets pop-up panel. This displays information on the
rounds in this feature and how they were created.
This feature has only one ‘set’ of edges.
The References section lists the edges
that were originally selected and is
where the failed edge(s) will be shown
with a red dot.
14. Scroll to find entries with a red dot and right click.
15. In the floating menu select Remove.
16. Repeat this for all entries with red dots.
17. Once all the failed
edges have been
deleted the green
lines showing the
round width will be
visible in the model
and the green tick in
the dashboard will be available.
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18. Click on the green tick
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.
The Menu Manager will now be asking you to confirm
the changes.
19. Click on Yes and the model should regenerate
successfully.
Adding a sketch reference.
The regulations state there must be at least 3mm of balsa surrounding the hole. We will
add a dimension constraint to make the shape 4mm above the hole to allow some
material for sanding. However, if you tried to create the dimension now you would not
be able to select the edge of the CO2 canister hole. To do this we need a sketch
reference.
20. In the main toolbar, click on
to change the view to Hidden Line.
You can now see the CO2 canister hole.
21. In the model tree expand the extrude that
created the side profile cut. This should be
Extrude 1.
22. Right click over the internal sketch and from
the floating menu select Edit Definition.
23. In the main toolbar, open the Sketch pulldown text menu and select References…
The References dialog will open showing existing
references.
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24. In the graphics window click on the top
horizontal line X1 of the CO2 canister
hole.
A dashed reference line will be created and a
new reference is added to the dialog.
X1
There is also a new dimensional constraint
between the new reference and the green line
above. This will be changed in the next
section.
25. Click
references.
to finish adding
Create a dimension constraint
Remember the dimension constraint you added to change the length of the nose? Here is
an explanation of the different types of dimension constraint.
There are four types of sketch dimension;
•
Locked – the dimension is locked to its value. This value cannot be modified either
directly or indirectly. The dimension has to be un-locked before its value can be
modified.
•
Strong – the dimension can be modified but only directly by the user
•
Weak - the dimension can be modified directly (by explicitly changing the value)
or indirectly (by changing other surrounding dimensions/geometry).
•
REF – the dimension is reporting a distance or size without controlling the sketch in
any way
Dimensions can be converted between these types.
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Changing the dimension constraint
26. Double click on the 9.4 mm constraint.
27. Change the value to 4 mm then press
Enter on the keyboard.
The dimension will change value, the line
will move and the dimension will now be
coloured Orange to show it is a strong
dimension and locked.
Before we close the sketcher we need to
restore the thickness of the nose to prevent
subsequent features failing.
28. Change the view to Shaded
.
29. In the Sketcher toolbar use
to add
the vertical dimension shown here and
change the value to 15 mm.
The model will regenerate and display the
new shape.
We now have a much sleeker body shape.
This should be faster for two key reasons.
°
The frontal area is less
°
Smaller size means reduced mass.
31. Save your model
What have you learned?
Having completed this session you should now:
Be aware:
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•
that Pro|ENGINEER can report the properties of components.
•
that Pro|ENGINEER allows the user to modify parts very easily.
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Understand:
•
how critical dimensions and geometry in parametric 3D models can be used to
modify the design.
Be able to:
•
assign component information including material properties to a model.
•
change a design by altering dimensions and geometry.
Session five – Assembly
Aim:
You will add combine your car body design and standard components to create an
assembly of the finished car.
Objectives:
By the end of the session you should:
Be aware
•
how Pro|ENGINEER combines components to form an assembly.
Understand
•
how component parts are brought together using assembly and/or mechanism
constraints to form an assembly
Be able to
•
start a new assembly and add components using constraints.
•
move the wheels kinematically on screen.
Focus:
During this session you will be shown how to start a new assembly file, add components
and locate them using assembly and mechanical constraints. The finished model will look
like the finished car and the wheels can be turned on screen.
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Introduction
Wheels and axles have been provided and together with your body design these will
create an ‘assembly’. Unlike Pro|DESKTOP, Pro|ENGINEER uses a different file
extension (ASM) for assembly files.
Task one - New assembly with fixed car body
create a New File.
to
2. In the New dialog choose Assembly
3. In the Name field type a name for the
assembly.
4. Click
An empty assembly will open in the
graphics window. The window may
appear empty.
5. If so, in the main toolbar click
make workplanes visible.
to
Notice the datum plane names for an
assembly have the prefix ASM_
Add a part
On the right of the graphics window, assembly tools have
been added to the toolbar.
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6. Click on
tool.
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the Add component…
7. The Open dialog opens
8. In your personal storage folder (Your
teacher will direct you to this) select
your car body file.
9. Click on
10. Your car body will be placed
temporarily in the graphics window
shaded a mustard colour and the
assembly dashboard will appear along
the bottom of the screen.
The dashboard is a very clever technique Pro|ENGINEER uses to present complex options
in a simple and easily understandable format.
11. In the dashboard, change the list currently showing Automatic to Fix.
12. Click on
the body.
to complete assembling
The dashboard closes and the body is fixed
in place, returning to its normal balsa
colour.
We can now add the axles.
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Task two - Assemble rear axle
1. Click on
to add another
component.
2. Locate and select the file
rear_axle_assy.asm
3. Click on
It is good practice to manoeuvre
the components close to their
required position before applying
assembly constraints.
These are the keyboard mouse
combinations that allow you to
manipulate components during
placement.
Pro|ENGINEER - Wildfire 3 - Quick reference
4. Manoeuvre the rear axle to the rear
of the body.
X1
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X1
5. Zoom in on the rear of the car
6. Make datum planes visible.
7. Click to select the small datum plane
X1 in the centre of the rear axle
named FRONT.
X2
8. Click to select the FRONT datum
plane in the body component X2.
9. The axle will move to line up the two
workplanes making them ‘co-planar’.
Note: If the wheels were not close enough
to their final position Pro|ENGINEER may
try to create an offset constraint.
If this is the case then do the following
otherwise skip to bullet 26.
10. In the assembly dashboard at the
bottom of the screen click on
Placement.
11. The Placement panel will open.
12. Change the Offset value to
Coincident.
13. Click on New Constraint.
Pro|ENGINEER should now be offering
you a new Automatic constraint.
14. Zoom in and select the outer
cylindrical surface of the rear axle.
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15. Zoom out and select the hole in the
body for the rear axle.
16. Check the Placement panel to make
sure the Allow Assumptions option is
NOT ticked.
An Insert constraint has moved the rear
wheels into position.
in the dashboard to
17. Click on
complete assembly of the rear axle.
The rear wheels are now in position.
Task three – Assemble front axle
1. Use the same steps to add
the front_axle_assy.asm
2. Save your design.
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Task four – Kinematic movement
Once assembled, components can be moved on screen providing they are not fully
constrained. Remember when adding the axle sub assemblies we made sure the Allow
Assumptions was not selected? This should allow the wheels to rotate. The technique we
will use to show movement is called ‘Kinematic’ motion.
Kinematic - The branch of mechanics that studies the motion of a body or a system of bodies
without consideration given to its mass or the forces acting on it. www.dictionary.com
There are two ways to move objects on screen. One uses the Drag (glove) tool and the
other uses keyboard/ mouse buttons.
Drag tool
Now for the exciting bit!
1. Click on
, the Drag… tool.
2. Click on one of the edges on the wheel.
A small diamond symbol appears at the
location where you clicked.
3. Click and hold the left mouse button and
drag to rotate the handle.
4. The mechanism should ‘operate’ on
screen. This is called Kinematic
movement.
In the top right corner of the computer screen
is the Drag dialogue.
5. To finish dragging, click on
the the Drag dialog.
in
Keyboard/ mouse buttons
6. Hold down the Ctrl + Alt keys on the
keyboard, move the mouse over a component
then click and hold the left mouse button to
drag the component.
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7. Save your model.
What have you learned
Now you have completed this session you should:
Be aware
° how Pro|ENGINEER combines components to form an assembly.
Understand
° how component parts are brought together using assembly and/or mechanism
constraints to form an assembly
Be able to
° start a new assembly and add components using constraints.
° move the wheels kinematically on screen.
Lesson six – Surface finishing own design
Aim:
You will use filler and abrasive paper to make the surface of the car body smooth and
then paint or varnish the surface the give a smooth, aerodynamic surface.
Objectives:
Be aware of
•
the need for smooth surfaces where aerodynamic efficiency is important.
•
of finishing techniques and how they contribute to better performance through
improved aerodynamics.
Understand
•
the concepts behind surface finishing and the need to preserve the designed
shape by minimising surface preparation.
•
how fillers, abrasive paper and paints can be used to produce a smooth flat
surface on timber.
Be able to
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•
to work safely when sanding their car body and applying surface finishes.
•
to achieve a finished car body that closely matches the design intent with a high
standard of finish.
Focus:
This is a workshop/ modelling studio session where you will be taught and have the
opportunity to apply techniques of filling, smoothing and finishing producing a surface on
the car body that will be aerodynamically efficient.
Lesson seven – Testing own design
Aim:
You will use a combination of Computational Fluid Dynamics (CFD) software and/or
actual testing of prototype designs to test the effectiveness of your design.
Note: CFD analysis requires the Schools Advanced Edition of Pro|ENGINEER and
additional CFD software.
Objectives:
Be aware
•
of the range of testing that can be applied to their car design.
•
how CFD software can be used as a virtual wind tunnel to test the aerodynamic
efficiency of 3D computer models.
Understand
•
the link between testing, analysis and improving designs in the light of testing.
•
how to carry out fair tests using rigorous scientific methods.
•
how to simplify and set-up 3D models in CFD software.
Be able to
•
set-up and carry out track tests on their designs using scientific method to control
variables and record results.
•
use the measurement tools in Pro|ENGINEER to analyse designs for
compliance with competition rules.
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•
interpret the results of testing and formulate suggested improvements based on
the results and an understanding of the competition rules.
•
suggest design improvements based on testing.
Focus:
A separate tutorial has been produced by Honeycomb Solutions for those schools that
have access to CFD software. With this you will be able to carry out aerodynamic
analysis of your design. www.honeycomb.ie
You should have access to testing your prototype and using the results to suggest design
improvements.
Lesson eight – Refine own design
Aim:
You will use the results of testing to make modifications that improve the performance of
your car designs.
Objectives:
Be aware
•
of the ease with which Pro|ENGINEER designs can be modified to produce
design variations on an initial design.
•
how the results of testing and an understanding of the competition rules and
vehicle efficiency are combined to suggest design improvements.
Understand
•
the concepts and principles of feature based parametric 3D modelling.
•
how to interpret the results of testing and use this to suggest design
improvements.
Be able to
•
edit the model tree for their car design, make changes and update the model.
•
use expertise with Pro|ENGINEER developed previously to alter their designs.
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•
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resolve feature failures with help from their teacher mentor.
Focus:
You should be able to use your new found Pro|ENGINEER skills to amend your design
incorporating the sessions gained from testing. The new designs can then be tested using
CFD/actual prototypes.
Lesson nine – Finish own design + Technical drawing
Aim:
In this session you will have the opportunity to finish your own design ready for CNC
manufacture in the next session.
For homework you will use a self paced tutorial to learn how create an engineering
drawing for your car design using Pro|ENGINEER.
Learning objectives:
Be aware
•
that CNC models must be finished to produce a final product.
•
of the international standards for engineering and technical drawings.
Understand
•
Understand the concepts behind surface finishing and the need to preserve the
designed shape by minimising surface preparation.
•
how technical drawings are used for quality control, assembly and operation of
products.
Be able to
•
Be able to work safely when sanding their car body and applying surface finishes.
•
Be able to achieve a finished car body that closely matches the design intent with a
high standard of finish use Pro|ENGINEER to create your own design of car
body.
•
use Pro|ENGINEER to create an orthographic drawing of your CO2 car including
a pictorial view.
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Focus:
During the school session you will have access to a PC running Pro|ENGINEER. You are
expected to model a car body of your own design by modifying the designs you have
created or by creating a model from scratch.
Homework:
An effective method of communicating designs to other people is via the use of drawings.
Pro|ENGINEER allows Designers and Engineers to quickly produce engineering
production drawings directly from the solid model.
To help engineers interpret drawings anywhere in the world standards for presentation
have been created. Historically every country had its own set of standards such as British
Standards but these have been refined to the major continents. Examples include ISO
widely used in Europe and the far east and ANSI from North America. In future we may
end up with one set of global drawing standards. Pro|ENGINEER can format drawings
for any international standard.
In the past, paper drawings have been the traditional method of communicating product
design information for manufacturing but the use of solid modelling has allowed a more
direct and automated link.
Using drawings requires the engineers to interpret 2D orthogonal views whereas the 3D
solid model contains more information and is easier to visualise. The use of Computer
Numerically Controlled (CNC) machines now allows engineers to produce components
directly from the solid model.
This level of automation means that orthographic drawings are now only being used to
provide overall dimensions, assembly details and inspection information.
In this section you will learn how to produce a detailed drawing of the CO2 car.
Task one - Creating a drawing
1.
Your car assembly must be open in Pro|ENGINEER.
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2.
From the Pro|ENGINEER top toolbar leftclick Create New File . In the dialog
box that appears the default Type is Part,
left-click Drawing. Enter the name of
your car. We will use Car_01.
3.
Notice the “Use default template” option
is checked. This will automatically create
views which have been pre-defined within
the default template file. We will use this
option to get a drawing quickly.
4.
Left-click
CO2 dragster
.
Note: If you want to learn how drawing views
are created in Pro|ENGINEER a good
starting point is the Sports drink bottle
project.
5.
In the New Drawing dialog that appears,
Pro|ENGINEER is giving you the option
of selecting which model is to be used
within the drawing.
6.
Your car assembly should be listed in the
Default Model field.
7.
In the Specify template section use the
default option - Use template.
8.
For the Format make sure a3_template is
selected. If not, use the Browse option to
browse to the drawing template directory,
select A3_FORMAT and click
.
9.
Left-click
to accept these settings
and create the drawing.
10. Pro|ENGINEER will create an A3
drawing with drawing border/format
and three orthographic views
Notice that the toolbar on the right of the
screen has changed to display the
commands and options relevant to drawing
creation.
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The views are too small so the scale of the drawing will be changed. Look in the bottom
left corner of the drawing area and you will see the current scale is set to 0.333.
This will be changed to 0.5
Changing the scale
1. Double click on the scale text at the
bottom of the drawing area.
2. A small dashboard will open at the very
bottom of the screen.
3. Alter the value to 0.5 then click on
.
The views are now larger and the scale text
shows the new value.
Adding centre lines
With three views in place we can add dimensions and annotations to the drawing.
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11. From the drawing toolbar select Show/Erase
This will open the Show/Erase dialog box.
.
The first step is to show the centre lines for the wheels.
12. In the Type section of the Show/Erase dialog left-click
Axis
.
Note: Clicking on buttons in the Type section toggles them
on/off.
13. In the Show By section make sure Feature is selected.
14. Roll the mouse wheel to zoom in on one of the views.
15. Move the cursor over one of the views.
16. Move the mouse over one of the wheels and when the
cylindrical surface making up the tyre pre highlights
click to select the wheel.
17. Pro|ENGINEER will create centre-lines indicating the
axes of the wheel revolve feature.
18. Select each wheel in the three views in turn until all
wheels have centre lines.
19. In the smaller Select dialog box select
.
This informs Pro|ENGINEER you have finished your
selections and will change the options in the Show/Erase
dialog.
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20. In the Show/Erase dialog select
by
, followed
.
Pro|ENGINEER will have created centre-lines in all 3 views.
To improve the aesthetics of the newly created centre-lines the length of the centre-lines
can be manually adjusted.
21. In the lower view select one of the newly
created centre-lines.
The centre-lines will now have drag handles at
each end.
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22. Using these drag handles drag the centrelines to the required lengths, and repeat
this process for the other centre-lines in
this and the other views.
Centre lines normally extend beyond the model
or main feature
Task two - Adding dimensions
The next step is to create dimensions. It is important to know the purpose of the drawing.
This could be to make the component, describe how to assemble the design or check
dimensional accuracy for quality control. For each of these the dimensioning scheme
would be different.
For our CO2 car the drawing will be used to show compliance with the competition
regulations. The key dimensions from the 2006 regulations for Ireland are:
Body dimensions
No
Structure
Min
Max
200
300
-
75
3a
Full body length
3b
Body height including wheels
3c
Body width at axles, front & back
35
42
3d
Total body width, including wheels
-
90
55
-
Body weight without CO2 cartridge (grams)
All dimensions stated in millimetres, mm
Official wheels must be used without modification and wheels must be 100% visible from
plan, side and end views.
CO cartridge dimensions
No
Structure
Min
Max
6a
CO2 cartridge diameter
19
20
6b
Lowest point of chamber to the race surface
26
40
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6c
Depth of hole
50
60
6d
Wall thickness around cartridge
3
-
All dimensions stated in millimetres, mm
Note: These tables have been reproduced from information on the official competition
website. http://www.f1inschools.ie/public/index.html
Details were correct at the time of writing but you must check with official sources and not
rely on these figures for your design or competition entry.
Pro|ENGINEER has the facility to import dimensions from the 3D model but for this
exercise we will create dimensions individually.
First you will dimension the width of the front wing.
Plan Dimensions
1.
In the sketcher toolbar on the right of the screen select
tool.
2.
Zoom in on the front of the car in the plan
view.
3.
Move the mouse cursor over the outside edge
of the front wing. When it pre-highlights in
cyan, click to select X1 and the edge will turn
red.
4.
Click on the other outside edge X2 of the front
wing to select it.
5.
Move the mouse cursor away from the model
into a clear space on the screen in front of
the car nose and middle mouse click to locate
the dimension text.
6.
The dimension will be created.
7.
Add another dimension for the widest part of
the wheels.
8.
Do the same at the rear of the car in the plan
view.
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, the Create dimension…
X1
X2
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Front view diensions
9.
In the front view, zoom in on the rear of the
car.
10. Create a dimension from the top of the car X1
to the bottom of the wheel X2.
11.
X1
X3
Click X3 to locate the dimension text.
The dimension text will not appear.
The prompt area at the bottom of the screen will
ask you to…
X2
A menu manager menu will be
visible in the top corner of the screen.
12. Click on Tangent and the
dimension will be created.
13. Add a body length dimension
to the front view.
14. Dimension the distance from
the bottom of the canister hole
to the bottom of the wheel.
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CO2 cannister hole
15. Zoom in on the end view for this section.
16. In the main drawing toolbar select
Show/Erase dialog tool.
the
because we will be revealing
17. Click on
dimensions from the model.
18. Click on
dimension.
to show we will be creating a
19. A Select dialog will appear.
20. In the drawing, click on the edge
of the canister hole.
The dimension will preview in blue.
21. Click
in the Select dialog.
22. In the Show/Erase dialog click on
then
to finish.
The diameter dimension has been created.
Quality control
The first session in this module helped you become familiar with the competition
regulations. One of the reasons manufacturing companies create drawings is to check
critical dimensions against the product specification. You can now do this for the car
design.
23. Compare the sizes for this model with the regulations.
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Can you see any that do not comply? If so, how could the model be changed to ensure it
meets the regulations? If you were to make changes to the model the drawing would
update automatically.
You have used the drawing to check the design against set criteria. This is a form of
‘quality control’.
Task three – Pictorial view
Additional views can be added at any time. In the steps that follow we will insert a
Trimetric shaded view to the drawing.
1.
Open the Insert pull-down menu,
select Drawing View then click on
General.
The Select Combined State dialog opens.
2.
Make sure No Combined State is
selected then click
.
The text area at the bottom of the screen is prompting you to Select CENTER POINT for
drawing
3.
On the drawing, click where you want the view. For example in the blank area
above the title block.
The Drawing View dialog opens
and the view previews in the
drawing.
In the Categories panel View
Type should be selected.
4.
In the Model view
names panel select
Trimetric from the list.
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5.
Click on
6.
The model orientation in
the drawing view will
change.
CO2 dragster
.
View display
7.
In the Categories panel
select View Display
8.
In the Display Style list
choose Shading.
9.
Click on
.
The view will now be shaded.
10. Click on
to
finish with the Drawing
View dialog.
Moving the view
The view may need to be
repositioned.
11. Click on the view to
select it.
A red rectangle will appear
when the view is selected.
12. Make sure the mouse cursor is over the selected view.
13. Hold down the right mouse button and, from the floating menu, click to deselect
Lock View Movement.
14. The view can now be dragged into position.
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Task four - Adding notes
The note tool in Pro|ENGINEER allows you to add text to the drawing. We will use it to
fill-in the title block.
1.
Zoom in on the title block in the
bottom right hand corner of the
drawing.
Notice some information has been
entered for you automatically. This
includes the drawing number from the
filename and the drawing scale.
Pro|ENGINEER can automate far more.
We will edit an existing, empty note and
then add a note manually.
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Edit an existing note
2.
Move the mouse inside the TITLE
rectangle and when it pre-highlights
click to select it.
The outline will turn red.
3.
Keep the mouse cursor inside the
selected rectangle then click and
hold the right mouse button.
4.
From the floating menu select
Properties.
The Note Properties dialog opens.
5.
Under the Text tab, delete any text
and type in CO2 Dragster.
6.
Click on
7.
The title block will now contain your
text.
.
Adding a note manually
8.
Open the Insert pull-down text menu and select Note…
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A NOTE TYPES menu manager dialog will open on the right of the
screen.
Selections are made in each section working from top to bottom.
9.
We will use the defaults so at the bottom click on Make Note.
The prompt at the bottom of the screen is telling us to:
10. Locate the large rectangle to the right of the orthographic
symbol.
11. Click near the top left corner of this rectangle X1.
X1
The prompt area at the bottom of the screen is waiting for you to type text for the note.
12. Type in the name of your team, we have used Flamerider.
13. Press ENTER on the keyboard
14. Type in F1 in Schools for a second line of text.
15. Press ENTER on the keyboard
16. Type in your school name or country, we have used Ireland.
17. Press ENTER on the keyboard twice.
18. Click on Done/Return to close the menu manager.
Your title block should now look something like this.
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19. Save your drawing and close down Pro|ENGINEER.
What have you learned
Now you have completed this session you should:
Be aware
•
of the international standards for engineering and technical drawings.
Understand
•
how technical drawings are used for quality control, assembly and operation of
products.
Be able
•
to use Pro|ENGINEER to create an orthographic drawing of your CO2 Car
including a pictorial view.
Lesson ten – Rendered image
Aim:
In this session you will be introduced to the Advanced Rendering Extension (ARX) module
of Pro|ENGINEER . With this you will be able to create photo-realistic images of your
models and assemblies.
Be aware of
•
the advanced rendering tools available in Pro|ENGINEER.
Understand
•
the basic concepts behind creating rendered images from models and
assemblies.
•
the key concepts and procedures in creating high quality photo-realistic
rendered images of their designs.
Know how
•
rendered images are used in a variety of commercial contexts.
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Be able to
•
place a model in a rendering environment.
•
create a rendered image of their design using a scene provided for them.
Task one - Getting started
1. Log-on and start Pro|ENGINEER
Key principles
The Advanced Rendering Extension (ARX) module in Pro|ENGINEER is very powerful
with many adjustments possible to the room environment such as materials, lighting,
reflections, etc possible.
This session will provide a brief overview and hands-on experience of just a few features,
enough to produce a final rendered image of the CO2 car assembly.
The sequence you will work through is:
•
Open an assembly of the CO2 car assembly
•
Define initial render settings
•
Load a scene definition
•
Position the model in the room
•
Change view of model
•
Try an initial render
•
Perform the final render
•
Save the rendered image
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Set working directory
2. The Navigator window on the left of
the screen should be displaying folders.
3. Browse to the folder with your car
design in.
4. Right click over your folder and from
the floating menu select Set Working
Directory.
5. Open your own car assembly.
The car body should already have a balsa
appearance and the wheels a plastic
material texture.
As you work through the rest of this section
you will notice objects look like the material
they would be made of.
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Task two - Initial render settings
Open the render toolbar
6. On a blank area of the main toolbar hold
down the right mouse button and from the
floating menu select Render.
The render toolbar appears in the main toolbar
on the left of the screen.
7. Changing the display settings inside
Pro|ENGINEER will help improve the
quality of the image on screen.
8. Open the View pull-down menu, select
Display Settings and then Model Display
9. Select the Shade tab at the top.
10. Change the shade Quality to 10.
11. Tick the box for Small Surfaces and click
then
.
To provide a good preview of your model,
room and shadows turn on real-time rendering.
This will help when adjusting other appearance
settings later on.
12. From the Rendering toolbar select the Real-Time rendering icon
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You will see the model display update, showing real-time rendering like this.
Note: If you have a low specification PC and the screen updates slowly you may need to
leave real-time render switched off until you have set up the render and are ready to
preview the image.
Task three - Load scene
A number of scenes have been setup for you specifying the room, lighting and
environment effects and one of these will be loaded.
in the render toolbar or open
1. Either click on
the View pull-down menu, click on Model Setup
and select Scene Palette.
2. In the Scenes dialog open the File pull-down menu
and select Append.
3. Navigate to the folder where the parts for this
tutorial are stored.
8. Select the scene called Bright_white.scn
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4. Make sure the new scene is selected; it
will be bordered by red. If not, double
click on the scene in the dialog to select
it.
5. Click on the Preview>>> button and a
thumbnail will show what your scene
will look like.
6. Select the Save scene with model
option.
7.
the Scenes dialog.
You will not see the full effect of the
changes you are making until later.
The model is unlikely to be in a suitable
position relative to the room.
The scene file has changed the room shape
to cylindrical.
Task four - Position model in room
In this section you will orientate the model in the room locking them together.
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Orient the model
1. In the main toolbar click on the small
arrow next to
the Saved views
button.
2. From the list of saved views select
Front.
3. The model will re-orientate to be
square to the computer screen.
Orient the room
4. In the Render toolbar click on
to open the Room Editor.
5. In the room editor dialog select the Rotate tab.
6. Click on
to position the room square to the computer screen.
Lock model to room
7. Change the Room locked to: option to
Model.
Now when you change the view of the
model it will remain the correct way up in
the room.
The only other adjustments you may want
to make to the room are the position of the
ceiling, floor and walls.
Room settings
8. In the Room Editor dialog select the
Position tab.
9. Turn the spin wheel labelled ceiling
and the top of the room will move up
and down. Set it to be above the
model like this.
10. Alter the position of the floor to below
the model a small distance.
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11. In the main toolbar click on the small
arrow next to
the Saved views
button.
12. From the list of saved views select Top.
13. The model and room will re-orientate
on the computer screen.
14. If the room is too large use the Wall 14 spin wheels to reduce the room size.
15.
the Room Editor
Task five - Change view of model
1. Either use one of the saved views or use the middle mouse button to drag the model
into the position you would like to view it. Notice how the room stays oriented to the
model.
2. Use the middle mouse scroll wheel to zoom in and out.
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Task six - Render
Setting up render controls
The next step is to generate a draft
rendering. To do this we need to first set
some rendering parameters.
1. In the Render toolbar, select the
Modify rendering settings icon
.
The Render Setup dialog opens.
2. Change the Renderer option at the
top to PhotoLux.
3. Leave the quality set to Draft.
4. Change the other settings to those
shown here then Close the dialog.
5. Select the Render icon
from the
Rendering Toolbar.
You have just created your
first rendering!
You can now play with the
position and render each
time until you are happy
with the final image.
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Final render
6. Before saving the image open the Render Setup
dialog, change the quality to the highest setting
and re-render the model.
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Task seven - Save rendered image
1. Click
in the Render toolbar or click View >
Model Setup > Render Setup to open the Render
Setup dialog.
2. Click the Output tab.
3. Change the Render To option to JPEG or another
image format of your choice.
4. A file name with the appropriate extension
appears in the File Name box. Edit this giving
the file a name you will remember.
5. Tick the Show Image Border option.
6. Change the image Size to Custom.
7. Alter the Width & Height until the border
surrounds your model.
8. Hold down shift and drag with the MMB to
position the model in the frame.
9. Close the Render Setup dialog.
10. In the Render toolbar click on
model.
to render the
11. The image with be saved with the required file
name.
A JPG image file has been created in the working
directory of the rendered model
12. Save your model, exit Pro|ENGINEER and logoff the computer/network.
What have you learned this session?
At the end of this session you should now:
Understand
•
the basic concepts behind creating rendered images from models and assemblies.
Know how
•
rendered images are used in a variety of commercial contexts.
Be able to
•
place a model in a rendering environment.
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to apply a ‘scene’ to create a final rendered image.
•
Lesson eleven – Testing modified design
This is a repeat of the previous testing session.
Note: Computational Fluid Dynamics analysis requires the Schools Advanced Edition of
Pro|ENGINEER and additional CFD software.
Aim:
You will use a combination of Computational Fluid Dynamics (CFD) software and actual
testing of prototype designs to test the effectiveness of your design.
Objectives:
Be aware
° how CFD software can be used as a virtual wind tunnel to test the aerodynamic
efficiency of 3D computer models.
Understand
° how to simplify and set-up 3D models in CFD software.
° how to carry out fair tests using good scientific methods.
Be able to
° carry out CFD analysis of their design.
° set-up and carry out track tests on their designs using scientific method to control
variables and record results.
° interpret the results of testing and formulate suggested improvements based on
the results and an understanding of the competition rules.
Focus:
Repeat the CFD and physical testing of your modified design.
You should have access to testing your prototype and using the results to suggest design
improvements.
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Homework
You should complete your e-presentation ready for delivery next session.
Lesson twelve – Presentations
Focus
This session is set aside for all teams to deliver your e-folios showing how your designs
were conceived, developed and manufactured.
Be aware of
•
the range of design, testing and manufacture used by students in their class.
Understand
•
there are many different ways of meeting a set of design requirements and that
compromises are required to balance often conflicting requirements.
Be able to
•
present their design ideas, development and manufacture through a projected efolio.
Module review
Over the last few sessions you have learned many new things including:
Be aware:
•
Of the concepts of 3D parametric solid modelling using Pro|ENGINEER
•
Of aerodynamic testing using Computational Fluid Dynamics (CFD) software.
Understand:
•
The principles of 3D parametric solid modelling using Pro|ENGINEER
•
How 3D solid modelling software be used to refine designs including parts and
assemblies.
•
How CFD software simulates aerodynamics and can help with body design.
Be able to:
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•
Create 3D solid model components from scratch using extrusions with internal
sketches and rounds
•
Assemble components using assembly constraints
•
Carry out CFD analysis on your car design. Note: this requires Pro|ENGINEER
Schools Advanced Edition and additional software.
To become confident creating parts, assemblies, rendered images and technical drawings
you will need to practice these techniques.
Extension activities
Design Challenges
•
Reverse engineer simple hand-held products like mobile telephones, PDAs,
toothbrushes.
•
Design and model a pair of hair straighteners.
Pro|ENGINEER tutorials
Additional tutorials that extend the techniques introduced here include:
Technique
Tutorial
Part modelling, assembly, drawing
Sports Drink Bottle
Assembly, mechanisms, animation
Cam toy
Wind Sculpture
Part modelling, assembly, design, team
working, rapid prototyping.
RP Car
D:\PTCData\AA ProE\AA Curriculum\01-06 CO2 dragster\CO2 dragster car.doc
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Transcription

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