Tutorial Pro-Engineer

Tutorial Pro-Engineer

(Parte 1 de 3)

Introduction To Modeling

By D Cheshire Page 1 of 10


ProEngineer Wildfire2 is a computer aided design (CAD) program that is used to create models on a computer in three-dimensions. Since three dimensions are used the models mimic real parts in the way that they are constructed. The models are sometimes referred to as virtual parts since at the design stage they only exist within the computer. Most of the models made in ProEngineer Wildfire2 are termed solid models which implies that the computer has a full understanding of the solidity of the part i.e. the computer ‘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 to make complex shapes.

ProEngineer Wildfire2 is a fully parametric CAD program. This means that when a part is designed and modeled dimensions are assigned which define the part. If, at a later time, these dimensions are found to be unsuitable they can be easily changed and the modification will filter through the system wherever the part appears. This is particularly helpful when dealing with collection of parts (known as an assembly) since if a modification is made to a single part, the modification is carried throughout the assembly. A designer can also define relationships between parts. For example, in an engine, if the diameter of the piston is increased or decreased, the corresponding engine block can be defined such that it is automatically modified to match the specifications of the modified piston.

Using any CAD system complex models need to be built by combining simpler shapes. In ProEngineer Wildfire2 these simpler shapes are called features. Several features are combined to form a part. Using Figure 1 as an example the part shown diagrammatically is made up of four features as 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 form assemblies 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 concepts including creating parts, creating basic features, sketching and saving information. Before starting to work through this tutorial you need to be sitting in front of a computer which has access to ProEngineer Wildfire2 and be logged on. You tutor should have advised you of how to log in already.

Start ProEngineer Wildfire2 by double clicking on the icon on your desktop or from the START menu. The main application window should appear shortly.

FEATURE Extrude Block

FEATURE Extrude Holes

FEATURE Extrude Slot

FEATURE Extrude Hole

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 main graphics 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 the word New… This is the icon for the NEW command. You could choose this icon from the toolbar below the menu if you prefer. Generally in this tutorial the menu command is given but you will often find the icon more convenient so look out for them.

Figure 3 : The New Part Dialog Box

After choosing the new command a dialog box will appear as shown in Figure 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 which means the units of length will be millimetres and units of mass will be Newtons 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 datum planes and a coordinate system. So what are datum planes? As the word plane implies these are flat areas that can be used as references for defining parts of your model. In some case you can define models without any datum planes, in other cases they are essential. Many people choose to always have a basic set of default datum planes (like the ones in your model) defined as a starting point for their model. Datum planes are displayed 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 to distinguish between the two sides of the datum. If you looking exactly onto the 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 3 of 10

Figure 5 : Start of the Part

Now let’s start modelling. Figure 6 shows the finished model we are going to make – it is a child’s calculator. As with any model you make there are lots of options as to how to approach the modelling process. We will describe one approach here – but there are others. The model is made from a series of building blocks called features. In general try and use as few features as possible but also keep each feature as simple as possible.

Figure 6 : The Toy Calculator

The starting point for our calculator will be a simple rectangular block of material made by a technique called extrusion.


Choose INSERT > EXTRUDE from the menu. Note the icon for this command which also appears to the right of the screen – it is a very commonly used command. You should see a new toolbar appear like the one in Figure 7. This is called the dashboard and contains all of the options for the type of feature you are creating.

Figure 7 : The Dashboard

To start creating this feature click on the PLACEMENT menu in the dashboard – highlighted in red – then press the DEFINE button. The Sketch dialog appears. Notice that this dialog has many fields but the sketch plane option is highlighted in pale yellow awaiting your input. The sketch plane is a flat surface onto which you will draw your shape. Choose the datum plane TOP by clicking on it in the graphics window or in the browser. The other fields in the Shape dialog are filled in automatically so you don’t need to worry about them at the moment – just click on the SKETCH button.

The graphics screen will change to a black background looking directly on to the sketch plane, and the icons described in Figure 9 will appear. You should also see a References dialog. References are used by ProEngineer to locate dimensions. ProEngineer guesses at suitable references and in this case will have chosen the Right and Front datum’s as shown in the main graphics window by the dotted lines. This is a good choice in this case so you can CLOSE this dialog.

You are now ready to use sketcher. Choose the rectangle tool and draw the rectangle with two clicks as shown in Figure 8.

Figure 8 : Outline Sketch

First click on the horizontal reference

Second click about here on the screen

Introduction To Modeling

By D Cheshire Page 4 of 10

Figure 9 : Sketcher Commands

Your window should now look like Figure 8 but the numbers in the dimensions will be different. If the dimensions aren’t positioned exactly as in 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 dimensions are 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 fully define the feature ProEngineer has automatically added dimensions that define the SIZE. The values of the dimensions are determined by the size that you drew the original rectangle. You will also notice that constraints have been created. These are indicated by the small symbols next to each line. V stands for vertical and H stands for horizontal.

Now to set the size of the rectangle to the correct value, choose the selection 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 changed and the shape will change to the sizes entered. To end sketching press the 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 display option 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 use the mouse wheel for this too.

Figure 10 : First Feature

(Parte 1 de 3)