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Introduction To Modeling
By D Cheshire
Page 1 of 10
Introduction ProEngineer Wildfire2 is a computer aided design (CAD) program that isused to create models on a computer in three-dimensions. Since threedimensions are used the models mimic real parts in the way that they areconstructed. The models are sometimes referred to as virtual parts sinceat the design stage they only exist within the computer. Most of the modelsmade in ProEngineer Wildfire2 are termed solid models which implies thatthe computer has a full understanding of the solidity of the part i.e. thecomputer ‘knows’ where there is material and where there is empty space.Solid
modelers
use
commands
to^
construct
models
that
reflect
manufacturing techniques, such as extrude and cut, combining these tomake complex shapes.ProEngineer Wildfire2 is a fully parametric CAD program. This means thatwhen a part is designed and modeled dimensions are assigned whichdefine the part. If, at a later time, these dimensions are found to beunsuitable they can be easily changed
and the modification will filter
through the system wherever the part appears. This is particularly helpfulwhen dealing with collection of parts (known as an assembly) since if amodification is made to a single part, the modification is carried throughoutthe assembly. A designer can also define relationships between parts. Forexample,
in
an
engine,
if
the
diameter
of
the
piston
is
increased
or
decreased, the corresponding engine block can be defined such that it isautomatically modified to match the specifications of the modified piston.Using any CAD system complex models need to be built by combiningsimpler shapes. In ProEngineer Wildfire2 these simpler shapes are calledfeatures. Several features are combined to form a part. Using Figure 1 asan example the part shown diagrammatically is made up of four featuresas follows:-
1.^
A rectangular block of material is created.
2.^
Removing material from the block creates a slot.
3.^
Finally material is removed to form a large hole.
4.^
Material is again removed to make four small holes.
Later tutorials will explain how several parts can be combined to formassemblies as shown in Figure 1.
Figure 1 : The Structure of Models
Creating a Part In this tutorial we will introduce you to some basic modeling conceptsincluding creating parts, creating basic features, sketching and savinginformation. Before starting to work through this tutorial you need to besitting in front of a computer which has access to ProEngineer Wildfire2and be logged on. You tutor should have advised you of how to log inalready.Start ProEngineer Wildfire2 by double clicking on the
icon on your
desktop or from the START menu. The main application window shouldappear shortly.
PART
PART
PART
PART
FEATURE^ Extrude^ Block
FEATURE^ ExtrudeHoles
FEATURES
FEATURES
FEATURES
FEATURE^ Extrude^ Slot
FEATURE^ ExtrudeHole
ASSEMBLY
SUB ASSEMBLY
Introduction To Modeling
By D Cheshire
Page 2 of 10
Figure 2: ProEngineer Main Window
You will see the normal Windows features – menus, toolbars, a maingraphics area and on the left side a browser window.The next step is to create your first part. To do this use the menu FILE >NEW. As you click on this menu notice the small picture to the left of theword New… This is the icon for the NEW command. You could choosethis icon from the toolbar below the menu if you prefer. Generally in thistutorial the menu command is given but you will often find the icon moreconvenient so look out for them.
Figure 3 : The New Part Dialog Box
After choosing the new command a dialog box will appear as shown inFigure 3. Notice that the Part option is already checked and type in calculator
as the name of this part (Note : ProEngineer does not allow
spaces and other special characters in names).A^
second
dialog
will
appear
offering
different
options
for
parts
in
particular different units of measurement. Choose mmns_part_solid whichmeans the units of length will be millimetres and units of mass will beNewtons and click on the OK button.
Figure 4 : Part Options
Well done – you have made your first part!
The part contains some
features already. The browser on the left of Figure 5 shows 3 datumplanes and a coordinate system. So what are datum planes? As the wordplane implies these are flat areas that can be used as references fordefining parts of your model. In some case you can define models withoutany datum planes, in other cases they are essential. Many people chooseto always have a basic set of default datum planes (like the ones in yourmodel) defined as a starting point for their model. Datum planes aredisplayed as rectangles that are just big enough to enclose the model.They are given names by the system such as RIGHT, TOP and FRONT.You will see datum planes drawn in either brown or black. This is todistinguish between the two sides of the datum. If you looking exactly ontothe
edge
of
a
datum
plane
you
will
see
two
parallel
lines
drawn
representing the two sides of the plane
Introduction To Modeling
By D Cheshire
Page 4 of 10
Figure 9 : Sketcher Commands
Your
window
should
now
look
like
Figure
but
the
numbers
in
the
dimensions will be different. If the dimensions aren’t positioned exactly asin Figure 8 don’t worry, just choose the select tool
and click and drag
the dimension text to a new position. You will notice that the dimensionsare
drawn
in
grey.
This
indicates
that
they
are
so
called
‘weak’
dimensions.
Weak
dimensions
will
be
automatically
replaced
if
they
become unnecessary.The drawing you have made defines the SHAPE of the feature. To fullydefine the feature ProEngineer has automatically added dimensions thatdefine the SIZE. The values of the dimensions are determined by the size
that you drew the original rectangle. You will also notice that constraintshave been created. These are indicated by the small symbols next to eachline. V stands for vertical and H stands for horizontal.Now to set the size of the rectangle to the correct value, choose theselection tool
and double click on each dimension and type in the
required value from Figure 8.The dimensions will now be in yellow indicating that they have changedand the shape will change to the sizes entered. To end sketching pressthe
icon. To complete this first feature type 12 into the numeric field
of the dashboard (See Figure 7) and click the green tick
to finish.
To
see
this
block
in
all
its
glory
choose
the
command
VIEW
ORIENTATION > STANDARD ORIENTATION and try the different displayoption icons
. You can also look around your design – press
the middle mouse button and move the mouse to spin the model around.Middle mouse button and SHIFT key moves the model around the screen.Middle mouse button and CTRL key zooms into the model – you can usethe mouse wheel for this too.
Figure 10 : First Feature
Enter Select Draw Rectangles
Draw Arcs Draw Curves Use Edges as Drag Geometry
Draw Text Mirror Objects
Draw Lines Draw Lines Draw Fillets Draw Points Add Dimensions
Constraints
Trim
Leave Sketcher^ Quit Sketcher
Introduction To Modeling
By D Cheshire
Page 5 of 10
Lets make a another extrusion on top of the first. Choose the commandVIEW > ORIENTATION > STANDARD ORIENTATION to make sure youare viewing the model correctly then choose INSERT > EXTRUDE fromthe menu. Start to draw a new sketch as before by clicking PLACEMENTthen DEFINE. The sketch plane option in the Shape dialog option ishighlighted in pale yellow awaiting your input. The sketch plane for thisfeature is the large flat surface of the first extrusion (see Figure 11a) soclick on this surface in the graphics window. Now click on the SKETCHbutton.We need to define some extra references in the sketcher. References areused to locate dimensions but they also allow you to ‘lock’ your drawingsonto existing edges. Whilst the references dialog is open click on the fouredges of the original extrusion – you may just see some dotted linesappear on them (see Figure 11b). Now close the references dialog anddraw the rectangle shown in Figure 11c – you should notice the cursorlocking onto the edges. Change the dimension to 55 and exit sketcher byclicking on
Figure 11 : Second Sketch
To end sketching choose
and click OK in the Section dialog. To
complete this first feature type 3 into the depth field of the dashboard (SeeFigure 7) and click the green tick to finish.
Figure 12 : Second Feature
You should be getting the hang of extrusions by now but we will comeback to them later – there is more to learn. Rounds The
calculator
looks
like
a
brick
let’s
improve
its
appearance
by
smoothing off some of the edges. To do this we will use the INSERT >ROUND command. The dashboard for the round command will appear asshown in Figure 13.
Figure 13 : The Round Dashboard
The round command has some great functionality. In its simplest form youjust need to click on the edges you want rounded. Click on the edgehighlighted in red in Figure 14a and change the value to 5 and click thegreen tick to finish the round.
Introduction To Modeling
By D Cheshire
Page 7 of 10
goes
round
the
whole
model
because
all
the
edges
are
tangential
(smoothly joined).Also add a 2 round all around the top edge of the screen. Again you willneed two picks because of the sharp corner.
Figure 17 : More Rounds
Patterns That’s the main part of the calculator completed. Now it is time to addsome details. We will start by creating the buttons. You may be thinkingthat these are just circular extrusions and you would be right – but ratherthan drawing each one individually will make use of some of the repetitionfeatures in CAD. The golden rule of CAD is don’t draw anything twice ifyou can avoid it!We will start by drawing just one of the buttons. It is an extrusion of acircle.
The
sketching
plane
is
shown
in
red
in
Figure
18a
and
the
dimensions are shown in Figure 18b. The height of the extrusion is 1.5.
Figure 18 : Button Extrusion
Now for the clever bit! We will make multiple copies of this first buttonusing the PATTERN command. You need to select what you are going topattern first so click on the button in the graphics window – it should turnred.
Now
choose
EDIT
PATTERN.
The
dashboard
for
the
pattern
command will be displayed.
Figure 19 : Pattern Dashboard
There are several types of pattern. The one we need is dimension based.You should have noticed that the dimensions of the button feature aredisplayed for you. This is because the group of buttons will be made bemade by copying the first button and after each copy is made one of thedimensions used to make the feature will be incremented by a specifiedamount to move the copy into its new position. The questions are whichdimensions, how much is the increment and how many copies. This iswhat you need to define now.First let’s make 4 copies of the button along the phone. Click on the 20dimension. An edit box appears into which you should type the incrementfor the dimension after each copy is made. Type in 8 – in other wordsthere will be 8 between each button along the phone. You must press theEnter button on the keyboard for your entry to be properly recognised. Wesaid we wanted 4 buttons in this direction so type 4 into the second inputbox from the left in the dashboard – again you must press Enter.If you ended pattern definition now you would get four buttons copiedalong the phone. We want buttons along AND across the phone. If youlook at the dashboard you will see the 4
th^ and 5
th^ input boxes are identical
to the 2
nd^
and 3
rd^
which you have already filled in. The 4
th^
and 5
th^
input
boxes are for the second direction of copies.To start to define the second direction click in the 5
th^ (last) input box which
currently says
Click here to add item
. Now click on the 15 dimension and
type in -10 as the increment and press Enter. A negative value is requiredbecause the 15 dimension needs to decrease each time a copy is made.Type 4 into the 4
th^ input box and press Enter to make 4 copies. You have
now completed the input and can end by clicking on the green tick. If youhave got it right you should see a rectangular array of 16 buttons.
Introduction To Modeling
By D Cheshire
Page 8 of 10
Figure 20 : Completed Pattern
Let’s have a go at a second pattern. Let’s say this is a Speak-&-Tellcalculator so we need a microphone and speaker. The speaker will be aseries of small cuts below the screen. As with the buttons we will makeone cut then make a pattern of copies.The first cut can be seen in Figure 23. It is a circular cut which is offcentre. There are no planes or surfaces which can be used as a sketchingplane – so we will have to make a new datum plane before we start theextrusion.Choose INSERT > MODEL DATUM > PLANE. This command allows youto create a datum. A dialog is displayed. This is an intelligent dialog as thecommand changes dependant on what geometry you select. Click on theRIGHT datum in the main graphics window and the command assumesyou want to create a datum plane parallel to RIGHT but a distance away –type in a distance of 10 and click OK. A new datum DTM1 is created.Enter the INSERT > EXTRUSION command. The familiar dashboard isdisplayed.
Figure 21 : Extrude Dashboard
Enter PLACEMENT and DEFINE and pick the new datum DTM1 as thesketching plane. With the references dialog open create a reference byclicking on the top edge of the calculator and draw a 10 circle in line withthis reference as shown in Figure 22.
Figure 22 : Speaker Cut Sketch
Close sketcher and type a distance of 1 into the dashboard and choosethe remove material option
. Finally a new option – so far we have
been extruding from the sketch plane in one direction because the option has been active. Change this to
and the extrusion will go both
sides of the sketch plane. Click the green tick
icon to end the feature
creation.
Figure 23 : Speaker Cut
Now to make a pattern of this feature. This is a simpler pattern because itonly copies in one direction. In the browser window right click on the lastextrusion and choose PATTERN to pattern the slot. You should see thepattern dashboard. The left-most option will be set to DIMENSION. Thisoption creates a pattern based on dimensions. We used it for the keypad.If you tried to use this option for this pattern you would find there was not a
Introduction To Modeling
By D Cheshire
Page 10 of 10
Figure 27 : The Finished Microphone Sketch
Conclusion That is our model completed. This is a simple
representation
model as it
doesn’t have all of the parts defined correctly – there are no internals andthe keys are ‘stuck on’ rather than being a separate keypad stickingthrough from the inside. In later tutorials you will see how you could modelthis more accurately.To make the calculator more interesting you could have a go at modellingsome numbers/symbols on each key. Choose the top of the key as asketching plane for an extrusion and use the
icon in sketcher to
‘draw’ each number. Extrude them 0.5 above the keys so you can just seethem.
Review So what should you have learnt?
•^
How to create a new part
-^
How to create extrusions to add and remove material.
-^
How to sketch basic shapes.
-^
How to create edge rounds.
-^
How to create simple patterns.
Any problems with these? Then you should go back through the tutorial –perhaps several times – until you can complete it without any help.Next have a go at modelling the shapes below then move on to Tutorial 2where you will attempt another model which uses different feature types.
Figure 28 : Some Sample Models – Estimate the Dimensions
Note the gaps here
