Creating a Simple Object in Pro/E: An Introduction to Sketcher and Sketching, Manuais, Projetos, Pesquisas de Mecatrônica

Baixe Creating a Simple Object in Pro/E: An Introduction to Sketcher and Sketching e outras Manuais, Projetos, Pesquisas em PDF para Mecatrônica, somente na Docsity! Pro | ENGINEER ® W I L D F I R E ™ 4.0 Tutorial and MultiMedia CD Roger Toogood, Ph.D., P. Eng. SDC Schroff Development Corporation www.schroff.com PUBLICATIONS INSIDE: MultiMedia CD An audio/visual presentation of the tutorial projects Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 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. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 4 Creating a Simple Object (Part I) Figure 5 Default datum planes Figure 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 some hing 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. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 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. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 6 Creating 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 11 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, non- tangent 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 Sk tcher, 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 under- specified; 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. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 9 Figure 13 Defining the sketch plane and sketch orientation reference preference. Both features we will make here are extrusions: one will be a protrusion (which adds material) and the other is a cut (which removes material). Either of the two methods shown here can be used to create either protrusions or cuts; for either method, whether you add or remove material is determined by a single mouse click! In the first method, we invoke Sketcher first to create the cross sectional shape of the extrusion. This shape is defined in a sketched curve which becomes a stand-alone feature in the model. We then launch the extrude command, specifying the curve to define the cross section of the feature. In the second method, we do not create a separate curve but rather invoke Sketcher from inside the extrusion creation sequence. In terms of design intent, the first method would be used if the sketched curve was going to be used for additional features, for example an extrude and a revolve. The second method (creating the sketch within the feature) is the traditional mode of operation, and would be the method of choice if the sketched shape was to be used only in a single feature. Creating a Sketched Curve When we left the model last, the datum plane DTM3 was highlighted in red. If that is not the case now, use preselection highlighting to select it now. In the datum toolbar on the right of the screen, pick the Sketch Tool button. Be careful not to pick the datum curve button below it - that one will create a datum curve using sets of existing datum points, points read from a file, or using equations. If you accidentally pick the wrong button, you can back out with the Quit command. Setting Sketch Orientation The Sketch dialog window opens as shown in Figure 13. Since DTM3 was highlighted (in red) prior to the present command, it has been preselected as the Sketch Plane. It is now highlighted in the graphics window in orange. This is the plane on which we will draw the sketch. The view orientation has changed so that Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 10 Creating a Simple Object (Part I) 3 Your system may be customized to let you stay in a 3D orientation when sketching. This is the configuration setting sketcher_starts_in_2d set to No. 4Well, almost always. It is possible to sketch in 3D, in which case you can manipulate your view so that you are not looking perpendicularly at the sketch plane. We will not attempt that here. you are looking directly at DTM33. Two dashed lines represent sketch references that have been chosen automatically - these are the other datum planes seen on edge. A yellow circle is actually the “tail feathers” of a view direction arrow. Spin the orientation with the middle mouse button to see the arrow. The yellow arrow attached to the edge of DTM3 should be pointing back into the screen. This is the direction of view onto the sketch plane. The direction of view can be reversed by clicking on the yellow arrow or with the Flip button in the dialog window (Figure 13). Leave it pointing towards the back. In the dialog window, DTM1 is identified as the Sketch Orientation Reference, with the Orientation set to Right. What is all this about? The relation between the sketch plane and the sketch orientation reference generally causes a lot of confusion for new users, so pay attention! The meaning of the sketch plane is pretty obvious - it is the plane on which we will draw the sketch - in this case DTM3. Our view is always perpendicular to the sketch plane4. That is not enough by itself to define our view of the sketch since we can be looking at that plane from an infinite number of directions (imagine the sketch plane rotating around an axis perpendicular to the screen). The Orientation option list in the dialog window (Top, Bottom, Left, Right) refers to directions relative to the computer screen, as in “TOP edge of the screen” or “BOTTOM edge of the screen” and so on. We must combine this direction with a chosen reference plane (which must be perpendicular to the sketch plane) so that we get the desired orientation of view onto the sketching plane. In the present case, when we get into Sketcher we will be looking directly at the brown (positive) side of DTM3. So that the sketch is the right way up, we can choose either DTM2 to face the Top of the screen, or (as was chosen automatically for us) DTM1 can face the Right of the screen. Note that both DTM1 and DTM2 are both perpendicular to the sketch plane, as required. The direction a plane or surface “faces” is determined by its normal vector. The normal vector for a datum plane is perpendicular to the brown side. For a solid surface, the orientation is determined by the outward normal. Read the last couple of paragraphs again, since new users are quite liable to end up drawing their sketches upside-down! To illustrate the crucial importance of the reference plane, consider the images shown in Figure 14. These show two cases where the same sketching plane DTM3 was used, the same sketched shape was drawn, the same reference orientation TOP was chosen, but where different datums were chosen as the sketching reference. On the left, the TOP reference was DTM2. On the right, the TOP reference was DTM1. The identical sketch, shown in the center, was used for both cases (rounded end of sketch towards the top of Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 11 Figure 14 The importance of the sketching reference plane! Figure 15 Choosing references in Sketcher the screen). However, notice the difference in the orientation of the part obtained in the final shaded images. Both of these models are displayed in the default orientation (check the datum planes). Clearly, choosing the sketching reference is important, particularly for the base feature. Let’s continue on with creating the curve. Make sure the Sketch dialog window is completed as in Figure 13. Select the Sketch button (or middle click). To verify the meaning of the dashed orange lines, in the top pull-down menu, select Sketch > References This opens the References dialog window, Figure 15. In this window we can select any existing geometry to help Sketcher locate the new sketch relative to the part. In the present case, there isn’t Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 14 Creating a Simple Object (Part I) Table 2-2 Sketcher Toolbar Flyout Buttons Button Flyout Group Button Commands Line 5 Tan-Tan Line 5 Centerline Circle 5 Concentric 5 3 Point 5 3 Tan 5 Ellipse Tangent End 5 Concentric 5 Center 5 3 Tan 5 Conic Arc Circular fillet 5 Conic fillet Point 5 Coordinate System Use Edge 5 Offset edge Dynamic trim (delete) 5 Trim(extend) 5 Divide Mirror 5 Rotate 5 Move Helpful Hint From wherever you are in the Sketcher menu structure, a single middle mouse click will often abort the current command and return you to the toolbar with the Select command already chosen. Sometimes, you may have to click the middle button twice. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 15 Figure 20 Drawing the Sketch Figure 19 RMB pop-up menu in Sketcher Creating the Sketch Select the Line tool using one of the following three methods: • using the Line toolbar button on the right, OR • in the pull-down menus select Sketch > Line > Line, OR • hold down the right mouse button and select Line from the pop-up menu (Figure 19). You will now see a small yellow X which will chase the cursor around the screen. Notice that the X will snap to the dashed references when the cursor is brought nearby. While you are creating the sketch, watch for red symbols (V, H, L) that indicate Intent Manager is firing an internal rule to set up a constraint (Vertical, Horizontal, Equal Length). These symbols will come and go while you are sketching. The trick with Sketcher is to get Intent Manager to fire the rule you want, then click the left mouse button to accept the position of the vertex. Click the corners in the order shown in Figure 20. After each click, you will see a straight line rubber-band from the previous position to the cursor position: 1. left-click at the origin (intersection of DTM1 and DTM2) 2. left-click above the origin on DTM1 (watch for V) 3. left-click horizontally to the right (watch for H and L - we do not want L) 4. left-click straight down on DTM2 (watch for V) 5. left-click back at the origin (watch for H) 6. middle-click anywhere on the screen to end line creation When you are finished this sequence, you are still in Line creation mode (notice the yellow X on screen and the Line toolbar button). If you middle click again, you will leave that and return to Select mode - the same as if you picked on the Select button in the right toolbar, but much faster. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 16 Creating a Simple Object (Part I) Helpful Hints If you make a mistake in drawing your shape, here are some ways to delete entities: 1. Pick the Select tool in the right toolbar and left click on any entity you want to delete. Then either press the Delete key on the keyboard, or hold down the RMB and choose Delete. 2. If there are several entities to delete, hold the CTRL key down while you left click on each entity. Then pick Delete as before. 3. You can left-click and drag to form a rectangle around a set of entities. Anything completely inside the rectangle is selected. Use Delete as before. 4. Notice the Undo and Redo buttons on the top toolbar We will cover more advanced Sketcher commands for deleting and trimming lines a bit later. Figure 21 Completed sketch with weak dimensions The sketched entities are shown in yellow. Since we have created a closed curve, the interior of the sketch is shaded (see the Shade Closed Loops button in the top toolbar). Many features require sketches to contain only closed loops, so this is an easy way to verify that condition. At some point or other, you will create a sketch that you think is closed, but it will not shade. This usually means you have extraneous entities in the sketch (usually duplicated lines or edges). We will see an example of this in a few minutes. Note that we didn't need to specify any drawing coordinates for the rectangle, nor, for that matter, are any coordinate values displayed anywhere on the screen. This is a significant departure from standard CAD programs. We also didn’t need the grid or a grid snap function (although both of these are available if you want them). You can also sketch beyond the displayed edges of the datum planes - these actually extend off to infinity. The displayed extent of datum planes will (eventually) adjust to the currently displayed object(s). After you have finished the sequence above, Sketcher will put two dimensions on the sketch - for the height and width of the rectangle. These will be in dark gray, so may be hard to see unless you pass your cursor over them, but similar to those shown in Figure 21. For the first feature in a part, the numerical values of these dimensions are picked more-or-less at random (although they are in correct Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 19 7 This sketch could be used to create an extruded surface feature, but with overlapping surfaces, probably not a good idea. For an extruded solid, the feature would fail with an error message about requiring a closed section only. Figure 24 Sketched curve (a “measle”) appears where the overlapping line ends. This indicates an open (that is, unconnected) end of the sketch (note the Highlight Open Ends button in the top toolbar). Third, a weak dimension will appear for the new line. Although the geometry of the sketch appears visually correct, if we tried to use it to create a solid feature it would fail7. Now pick the Show Overlapping Geometry button in the top toolbar. All lines touching the offending vertical line will highlight in green. At this point, you would have to do some detective work to figure out where the problem was. Select the short vertical line (note that preselection works here) and delete it. The red measle disappears and the sketch is again shaded. You should experiment with the Sketch Diagnostic tools periodically as we proceed through the tutorial. Note that these are also available under Sketch in the pull-down menus at the top. This completes the creation of our first sketch. Select the Accept (or Continue) toolbar icon (the check mark). This returns us to the regular graphics window with our new sketched curve shown in red (last feature created). You can spin the mod l around with the middle mouse button to see this curve from different view points. When you are finished with this, return the model to approximately the default orientation - Figure 24. Creating a Solid Protrusion Most of the work to create this feature has been done already - creating the sketched curve that defines its shape. This curve should be highlighted in red. If you have been playing around with the model and the sketch is blue, just left click on it to select it again. There are a number of ways to launch the protrusion creation command. With the sketched curve highlighted, the easiest way is to pick the Extrude button in the right toolbar. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 20 Creating a Simple Object (Part I) Figure 25 The protrusion preview What you will see now is a yellow shaded image of the protrusion, Figure 25. On this shape, you will see a yellow arrow that indicates the extrusion direction, which by default comes off the positive side of the sketch. There is also a dashed line ending in a white square. This is a drag handle. Click on this with the mouse and you can drag it to change the length of the extrusion. This length is also shown in a dimension symbol. You can even drag this extrusion out the back of the sketch to extrude in the opposite direction. This direct manipulation of the feature on the screen is called, in Pro/E vernacular, Direct Modeling. Bring the protrusion out the front and double click on the numeric dimension, and enter the value 30. At the bottom of the graphics window is a new collection of tools. These comprise the Dashboard. Many features are constructed with tools arranged using this interface element. It is worth spending some time exploring this one in detail, since you will probably be using it the most. The Extrude Dashboard The dashboard collects all of the commands and options for feature creation in an easily navigated interface. Moreover, most optional settings have been set to default values which will work in the majority of cases. You can change options at any time and in any order. This is a welcome and significant departure from releases of Pro/E prior to Wildfire. The dashboard contains two areas. On the left (Figure 26) are commands, settings, and so on for the particular feature under construction. On the top row, the feature is identified with the toolbar icon - extrude in this case - and several slide-up panels which do the following: Helpful Hint You may accidentally leave the dashboard with an inadvertent click of the middle mouse button. Remember that this is a short cut for Accept. If that happens, with the protrusion highlighted in red, hold down the right mouse button and select Edit Definition. This will bring you back to the dashboard. The Undo command, if executed immediately, will delete the feature. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 21 Extrude Icon Thicken Sketch Remove Material Flip direction Blind depth Depth spec options Surface Solid Sketch plane and Sketcher Figure 26 The Extrude Dashboard Figure 27 Extruded surface Placement - allows you to select, create, or modify the 2D section t be used for the feature. Since we preselected the sketched curve, it is now listed on this panel. If we had not preselected the curve, we could have chosen it now, or launched Sketcher from this panel to create a new sketch. This would involve selecting the sketching plane, sketcher reference, and so on. We will go this route in the next feature. If you wanted to change the sketch for the extrude, this is how you access it. The Unlink button is currently displayed on the Placement panel. This button appears if, like now, you have preselected a curve to serve as the sketch for the extrude. Thus, the extrude is linked to the previous curve feature; changes to the geometry or dimensions of the curve would drive changes in the shape of the extrude. The curve itself is a separate entry on the model tree. The purpose of unlinking is to break this (parent/child) connection to the original curve. If you were to select this command (don’t do this now), a copy of the original curve will be brought into the extrude feature. In that case, a change to the original curve would not affect the extrude. The original curve could be modified, moved, or even deleted, and the extrude would still be able to regenerate. The use of external curves to drive feature geometry is an important aspect of an advanced modeling technique that makes use of skeleton models. Options - information about the depth specification for the feature. We will find out what is meant by “Side 2" in a later lesson. For a simple extrude, the depth specification is easiest to set using one of the icons in the lower dashboard area (see below). Properties - specify the name of the feature The icons on the second row operate as follows: Solid and Surface buttons - these are an either/or toggle set. The default button is to create a solid. If you pick the next button, Surface, the sketch will be extruded as an infinitely thin surface (Figure 27). Return this to the Solid selection. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 24 Creating a Simple Object (Part I) We will now add another extruded feature - this time we will create a cut that removes material. Furthermore, instead of creating the sketch first, as we did for the solid protrusion, we will create the sketch within the feature itself. This is actually the more common way to use Sketcher. Before we do that, now is a good time to save the part. Saving the Part It is a good idea when you are just getting started to save your model quite frequently, just in case something serious goes wrong. If you have to bail out of the program, you can always reload the most recently saved copy of the part and continue from there. There are (as usual!) several ways to save the part: • in the top toolbar, select the Save button, or • in the pull-down menus select File > Save, or • use the keyboard shortcut CTRL-S. Make sure that the Save Object dialog is showing the des red working directory at the top. If not, select it in the Common Folders area in the Navigator. At the bottom of the dialog window, the name of the current active object (remember that you can have more than one object loaded into memory at a time) should already be in view. Accept the default model name [block.prt] (this is the active part) by pressing the enter key or the middle mouse button. Pro/E will automatically put the part extension (prt) on the file. If you save the part a number of times, Pro/E will automatically number each saved version (like block.prt.1, block.prt.2, block.prt.3, and so on). Be aware of how much space you have available. It may be necessary to delete some of the previously saved versions; or you can copy them to a diskette. You can do both of these tasks from within Pro/E - we'll talk about that later. IMPORTANT NOTE: The Save command is also available when you are in Sketcher. Executing this command at that time will not save the part, but it will save the current sketched section with the file extension sec. This may be useful if the sketch is complicated and may be used again on a different part. Rather than recreate the sketch, it can be read in from the saved file (using Data from File). In these lessons, none of the sketches are complicated enough to warrant saving them to disk. Now we will proceed n to the next feature - an extruded cut. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 25 Sketching Plane Sketching Reference (TOP) Figure 32 Setting up to sketch the cut Sketch reference Sketch reference Figure 33 References for cut sketch Creating an Extruded Cut Start by launching the Extrude command from the right toolbar. The extrude dashboard at the bottom of the screen opens. Open the Placement slide-up panel in the dashboard and select Define. The Sketch dialog window appears. This time, however, nothing has been preselected for us as it was for the previous sketch. We’ll have to enter the data ourselves. First, the dialog is waiting for you to select the sketching plane (notice the pale yellow data entry field). Pay attention to preselection here. Notice the preselection filter setting (should be Surface); you will not be able to pick an ed e or a curved surface (both of these would be illegal). Pick on the right side surface of the block (see Figure 32). As soon as you pick the sketching plane (it highlights in orange), a yellow arrow will appear showing the default direction of view relative to the surface. The Flip button can be used to reverse this direction, but leave it as it is. Pro/E makes a guess at a potential reference plane for you to use. This may depend on the current orientation of your view, and might result in a strange view orientation in sketcher (like sideways or even upside down). We want to be a bit more careful and specific here. Pick on the top planar surface (Figure 32), between the two tangent lines of the rounded corners; the surface will highlight in red. In the Orientation pull-down list, select Top so that the reference will face the top of the screen. We now have our sketch plane and reference set up, so select Sketch at the bottom of the dialog window. We are now in Sketcher (Figure 33). Two references have been chosen for us (the back and top surfaces of the object). We are going to create the U-shaped figure shown in Figure 34. Note that there is no sketched line across the top of the U - there is no inside or outside. Thus, it is technically called an open sketch (as opposed to a closed sketch for our previous feature). There are some restrictions on the use of open sketches which we will run across in a minute or two. You might prefer to set your display mode to Hidden Line at this point. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 26 Creating a Simple Object (Part I) 1 2 3 4 Figure 34 Sketch geometry Use the RMB pop-up menu to select the Line command. Start your sketch at vertex 1 in Figure 34 - the cursor will snap to the reference. Then drag the mouse down and pick vertex 2 (note the V constraint), and middle click twice to end the Line command. Some weak dimensions will appear. Do nothing about them yet because, since they are weak, they are liable to disappear anyway. If we make them strong, this will cause us extra work dealing with Intent Manager. Use the RMB pop-up menu again and select the 3-Point/Tangent End command. Pick on the end of the sketched line (vertex 2) and drag the mouse downwards in the direction of tangency. Once the arc has been established, drag the cursor over to the right (the arc will rubber-band while maintaining the tangency constraint) and click at vertex 3. (If you drag straight across to vertex 3 you will get a 3-point arc which is not automatically tangent at vertex 2.) You should see two small blips that indicate when vertex 3 is at the same height as the center of the arc. Use the RMB menu to pick Line again. Now left click at vertex 3 and draw a vertical line up to snap to the reference at vertex 4, making sure that you have a tangent constraint (T) at vertex 3.. Our sketch is complete. Use the middle mouse button to return to Select mode. Your dimension values may be different from those shown in Figure 34. Your dimensioning scheme may even be slightly different. It will be easier to see this if you go to hidden line display instead of shading. All the dimensions should be weak. Drag them to a better location if necessary (off the part). Don’t be afraid to resize your display so that you can see everything clearly. Compare the dimensioning scheme with the one in Figure 35. We want to have a Helpful Hint In general, try to keep your sketches closed - you will have fewer problems that way. Helpful Hint Wait until the shape of the sketch is finished before you start worrying about the dimensioning scheme or dimension values. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 29 10 Model parameters and layers are discussed in the Advanced Tutorial. Figure 38 Removing from the wrong side of the sketch Figure 39 Cut feature completed We are finished creating this feature, so select the Accept button at the right end of the dashboard. The part should now look like Figure 39 when in default orientation. The cut will be highlighted in red as usual, as the last feature created. Save the part. We will need it in this condition for the next chapter. Using Part Templates You will recall that in the block part created earlier, the first thing we did was to create default datum planes. These (plus the named views based on them, which we didn’t create this lesson) are very standard features and aspects of part files, and it would be handy if this was done automatically. This is exactly the purpose of part templates. A template is a previously created part file that contains the common features and aspects of almost all part files you will ever make. These include, among other things, default datum planes and named views. Pro/E actually has several templates available for parts, drawings, and assemblies. There are variations of the templates for each type of object. One important variation consists of the unit system used for the part (inches or millimeters). Templates also contain some common model parameters and layer definitions10. A template can be selected only when a new model is first created. Let’s see how that works. Create a new part (note that you don’t have to remove the block - Pro/E can have several parts “in session” at the same time) by selecting File > New or using the “Create New Object” button. The New dialog window opens. The Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material 2 - 30 Creating a Simple Object (Part I) Part | Solid options are selected by default. Enter a new name, like exercise_1. Remove the check mark beside Use default tem late (we normally don’t do t is, but we should have a look at what is available) and then select OK. In the New File Options dialog window, the default template is shown at the top. It is likely “inlbs_part_solid” (unless your system has been set up differently). This template is for solid parts with the units set to inch-pound-second. It seems strange to have force and time units in a CAD geometry program. Actually, this is included so that the part units are known by downstream applications like Pro/MECHANICA which perform finite element analysis (FEA) or mechanism dynamics calculations. These programs are very picky about units! Note that there are templates available for sheet-metal parts and for metric units (millimeter-Newton-second). While we are mentioning units, be aware that if you make a wrong choice of units here, it is still possible to change the units of a part after it has been created (see Edit > Setup > Units). There are only two model parameters in the default template. DESCRIPTION is for an extended title for the part, like “UPPER PUMP HOUSING”. This title can (eventually) be called up and placed automatically on a drawing of the part using, you guessed it, a drawing template. Similarly, the MODELED_BY parameter is available for you to record your name or initials as the originator of the part. Fill in these parameter fields and select OK. The new part is created which automatically displays the default datums. They are even named for you (we will see how to name features in lesson 3): instead of DTM1, we have RIGHT. TOP replaces DTM2, and FRONT replaces DTM3. The part also contains a coordinate system, named views (look in the Saved Views List), and other data that we’ll discover as we go through the lessons. The named views correspond to the standard engineering views. Thus, it is important to note that if you are planning on using a drawing template, your model orientation relative to the default datums is critical. The top-front-right views of the part are the ones that will be automatically placed on the drawing later. If your model is upside down or backwards in these named views, then your drawing will be too. This is embarrassing and not likely to win favor with your boss or instructor! Now, having created this new part, you are all set up to do some of the exercises at the end of the lesson. Do as many of these as you can. Perhaps do some of them in different ways by experimenting with your sketch orientation, Sketcher commands, and so on. Copyrighted Material Copyrighted Material Copyrighted Material Copyrighted Material Creating a Simple Object (Part I) 2 - 31 This completes Lesson #2. You are strongly encouraged to experiment with any of the commands that have been presented in this lesson. Create new parts for your experiments since we will need the block part in its present form for the next lesson. In the next lesson we will add some more features to the block, discover the magic of relations, and spend some time learning about the utility functions available to give you information about the model.