Tutorial proengineer

Tutorial proengineer

(Parte 1 de 5)

Pro | ENGINEER® WILDFIRE™ 4.0

Tutorial and MultiMedia CD

Roger Toogood, Ph.D., P. Eng.

Schroff Development Corporation w.schroff.com

INSIDE: MultiMedia CD

An audio/visual presentation of the tutorial projects

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Creating a Simple Object (Part I)2 - 1

Lesson 2

Creating a Simple Object (Part I) Introduction to Sketcher

Synopsis

Creating a part; introduction to Sketcher; sketch constraints; creating datum curves, protrusions, cuts; sketch diagnostics; using the dashboard; saving a part; part templates.

Overview of this Lesson

The main objective of this lesson is to introduce you to the general procedures for creating sketched features. We will go at quite a slow pace and the part will be quite simple (see Figure 1 on the next page), but the central ideas need to be elaborated and emphasized so that they are very clearly understood. Some of the material presented here is a repeat of the previous lesson - take this as an indication that it is important! Here’s what we are going to cover:

1.Feature Types and Menus 2.Introduction to Sketcher <Sketcher menus

<Intent Manager and Sketcher constraints

< Sketcher Diagnostics 3.Creating a Datum Curve 4.Creating an Extruded Protrusion

<Using the Dashboard 5.Creating an Extruded Cut 6.Saving the part 7.Using Part Templates

It will be a good idea to browse ahead through each section to get a feel for the direction we are going, before you do the lesson in detail. There is a lot of material here which you probably won’t be able to absorb with a single pass-through.

Start Pro/E as usual. If it is already up, close all windows (except the base window) and erase all objects in session using File > Erase > Current and File > Erase > Not Displayed. Close the Navigator and Browser windows.

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2 - 2Creating a Simple Object (Part I)

Figure 2 Creating a new partFigure 1 Part at the end of this lesson

Creating a Simple Part

In this lesson, we will create a simple block with a U-shaped central slot. By the end of the lesson your part should look like Figure 1 below. This doesn't seem like such a difficult part, but we are going to cover a few very important and fundamental concepts in some depth. Try not to go through this too fast, since the material is crucial to your understanding of how Pro/E works. We will be adding some additional features to this part in the next lesson.

We are going to turn off some of the default actions of Pro/E. This will require us to do some things manually instead of letting the program do them automatically. This should give you a better understanding of what the many default actions are. Furthermore, eventualy you wil come across situations where you don’t want the defaults and you’l need to know your way around these options.

Creating and Naming the Part

Click the Create New Object short-cut button, or select File > New. A window will open (Figure 2) showing a list of different types and sub-types of objects to create (parts, assemblies, drawings, and so on). In this lesson we are going to make a single solid object called a part. Keep the default radio button settings

Part | Solid

IMPORTANT: Turn off (remove the check) the Use Default Template option at the bottom. We will discuss templates at the end of this lesson.

Many parts, assemblies, drawings, etc. can be loaded simultaneously (given sufficient

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Creating a Simple Object (Part I)2 - 3

1 Pro/E can keep track of objects of different types with the same names. A part and a drawing can have the same name since they are different object types.

Datum Axis Datum Plane

Datum Curve

Sketched Curve

Datum Point Coord System

Figure 4 Toolbar buttons for creating DATUMS

Figure 3 Options for new parts computer memory) in the current session. All objects are identified by unique names1. A default name for the new part is presented at the bottom of the window, something like [prt0001]. It is almost always better to have a more descriptive name. So, double click (left mouse) on this text to highlight it and then type in

[block]

(without the square brackets) as your part name. The Common Name of the part is an option for specifying an even more descriptive name. For example, you might have a number of part files named using a part or catalog number such as “TG123_A29". This is not very descriptive, so you could enter a common name such as “small flat rubber washer”. We will not use common names in this tutorial, so leave this blank and just press Enter or select OK.

The New File Options dialog window opens. Since we elected (in the previous window) to not use the default template for this part, Pro/E is presenting a list of alternative templates defined for your system. As mentioned previously, we are going to avoid using defaults this time around. So, for now, as shown in Figure 3 at the right, select

Empty | OK (or middle click).

At this time, BLOCK should appear in the title area of the graphics window. Also, some of the toolbar icons at the right are now “live” (i.e. not grayed out).

Create Datum Planes

We will now create the first features of the part: three reference planes to locate it in space. It is not absolutely necessary to have datum planes, but it is a very good practice, particularly if you are going to make a complex part or assembly. Datum planes are created using the “Datum Plane” button on the right toolbar, as shown in Figure 4. Note that these icons look quite similar to the buttons on the top toolbar that control the display of datums. What’s the difference?

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2 - 4Creating a Simple Object (Part I)

Figure 5 Default datum planesFigure 6 Datum planes as solid plates

Select the Datum Plane button now. Since we currently have no features in the model, Wildfire rightly assumes that we want to create the three standard datum planes.

The datum planes represent three orthogonal planes to be used as references for features that will be created later. You can think of these planes as XY, YZ, XZ planes, although you generally aren’t concerned with the X,Y,Z form or notation. Your screen should have the datum planes visible, as shown in Figure 5. (If not, check the datum display button in the top toolbar.) They will resemble something like a star due to the default 3D viewing direction. Note that each plane has an attached tag that gives its name: DTM1, DTM2, and DTM3. This view may be somewhat hard to visualize, so Figure 6 shows how the datum planes would look if they were solid plates in the same orientation. An important point to note is, while the plates in Figure 6 are finite in size, the datum planes actually extend off to infinity. Finally, before we move on to the next topic, notice that the last feature created (in this case DTM3), is highlighted in red. This is a normal occurrence and means that the last feature created is always preselected for you as the “object” part of the object/action command sequence.

Pro/ENGINEER Feature Overview

Below (and/or to the right of) the datum creation buttons in the right toolbar are three other groups of buttons. These are shown in Figures 7, 8, and 9. If you move the cursor over the buttons, the tool tip box will show the button name.

Two of these menus contain buttons for creating features, organized into the following categories:

Placed Features (Figure 7) - (holes, rounds, shells,) These are features that are created

directly on existing solid geometry. Examples are placing a hole on an existing surface, or creating a round on an existing edge of a part.

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Creating a Simple Object (Part I)2 - 5

Hole Shell

Rib Draft

Round

Chamfer

Figure 7 The Placed Features toolbar

Extrude

Revolve Sweep

Blend

Style

Figure 8 The Sketched Features toolbar

Mirror Merge

Trim

Pattern Figure 9 The Edit toolbar

Sketched Features (Figure 8) - (extrusions, revolves, sweeps, blends, ..) These features require the definition of a two-dimensional cross section which is then manipulated into the third dimension. Although they usually use existing geometry for references, they do not specifically require this. These features will involve the use of an important tool called Sketcher.

The final group of buttons (Figure 9) is used for editing and modifying existing features. We will deal with some of these commands (Mirror and Pattern) later in the Tutorial.

In this lesson we will be using the Extrude command to create two types of sketched features (a protrusion and a cut). In the next lesson, we will use the Hole, Round, and Chamfer commands to create three placed features. Before we continue, though, we must find out about an important tool - Sketcher.

Introducing Sketcher

Sketcher is the most important tool for creating features in Pro/E. It is therefore critical that you have a good understanding of how it works. We will take a few minutes here to describe its basic operation and will explore the Sketcher tools continually through the next few lessons. It will take you a lot of practice and experience to fully appreciate all that it can do.

Basically, Sketcher is a tool for creating two-dimensional figures. These can be either stand-alone features (Sketched Curves) or as embedded elements that define the cross sectional shape of some solid features. The aspects of these figures that must be defined are location, shape, and size, roughly in that order. The sketching plane where we will create the 2D sketch is defined or selected first. Then, within Sketcher the location is further specified by selecting references to existing geometry. You will find the usual drawing tools for lines, arcs, circles, and so on, to create the shape. Finally, you can specify alignments or dimensions to control the size of the sketch and its relation to existing geometry.

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2 - 6Creating a Simple Object (Part I)

2 Intent Manager was introduced several releases ago. Some veteran Pro/E users still have not made the switch from “the old days”. For those users, Pro/E has the ability to turn off the Intent Manager and let them do everything manually.

Figure 1 Geometry after processing by Intent Manager. Note aligned vertices, parallel edges, tangent curves.

Figure 10 Geometry input by user (Intent Manager off). Note misaligned vertices, non-parallel edges, nontangent curves.

Sketcher is really quite “smart”, that is, it will anticipate what you are going to do (usually correctly!) and do many things automatically. Occasionally, it does make a mistake in guessing what you want. So, learning how to use Sketcher effectively involves understanding exactly what it is doing for you (and why) and discovering ways that you can easily over-ride this when necessary.

The “brain” of Sketcher is called the Intent Manager. We will be discussing the notion of design intent many times in this tutorial. In Sketcher, design intent is manifest not only in the shape of the sketch but also in how constraints and dimensions are applied to the sketch so that it is both complete and conveys the important design goals for the feature. Completeness of a sketch implies that it contains just enough geometric specification so that it is uniquely determined. Too little information would mean that the sketch is underspecified; too much means that it is over-specified. The function of Intent Manager is to make sure that the sketch always contains just the right amount of information. Moreover, it tries to do this in ways that, most of the time, make sense. Much of the frustration involved in using Sketcher arises from not understanding (or even sometimes not realizing) the nature of the choices it is making for you or knowing how easy it is to override these actions. When you are using Sketcher, Intent Manager must be treated like a partner - the more you understand how it works, the better the two of you will be able to function2.

The term sketch comes from the fact that you do not have to be particularly exact when you are “drawing” the shape, as shown in the two figures below. Sketcher (or rather Intent Manager) will interpret what you are drawing within a built-in set of rules. Thus, if you sketch a line that is approximately vertical, Sketcher assumes that you want it vertical. If you sketch two circles or arcs that have approximately the same radius, Sketcher assumes that’s what you want. In cases like this, you will see the sketched entity “snap” to a particular orientation or size as Intent Manager fires one of the internal rules.

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Creating a Simple Object (Part I)2 - 7

Figure 12 A sketch showing implicit constraints

When Sketcher fires one of its internal rules (this occurs on-the-fly while you are sketching), you will be alerted by a symbol on the sketch that indicates the nature of the assumed condition. If you accept the condition, it becomes a constraint on the sketch. These constraint symbols are summarized in Table 2-1 on the next page. You should become familiar with these rules or constraints, and learn how to use them to your advantage. If you do not want a rule invoked, you must either (a) use explicit dimensions or alignments, or (b) exaggerate the geometry so that if fired, the rule will fail, or (c) tell Sketcher to disable a specific instance of the constraint (Hint: RMB), or (d) set up Sketcher to explicitly ignore constraints of a given type.

You will most often use option (a) by specifying your desired alignments and dimensions and letting Sketcher worry about whatever else it needs to solve the sketch. When geometry is driven by an explicit dimension, fewer internal rules will fire. Option (b) is slightly less common. An example is if a line in a sketch must be 2E away from vertical, you would draw it some much larger angle (like 15E or so) and put an explicit dimension on the angle. This prevents the “vertical” rule from firing. Once the sketch has been completed with the exaggerated angle, you can modify the dimension value to the desired 2E. The third option is used while you are sketching to disable a constraint that Intent Manager indicates it wants to place. Finally, there are settings for Sketcher that explicitly turn off the rule checking (for all rules or selected ones only) during sketching. This is very rarely used.

An example of a sketch with the geometric constraints is shown in Figure 12. Note how few dimensions are required to define this sketch. See if you can pick out the following constraints:

<vertical lines <horizontal lines

< perpendicular lines

< tangency

<three sets of equal length lines <equal radius

<vertical alignment (two cases)

How do you suppose Sketcher is able to determine the radius of the rounded corners (fillets) at the top and bottom on the left edge? (Hint: this involves the solution of a system of equations.)

(Parte 1 de 5)

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