Lesson 4 Holes and Rounds 111 Figure 4.1 Breaker OBJECTIVES Sketch arcs in sections Create a straight hole through a part Complete a Sketched hole Understand the Hole Tool Use Info to extract information about the features and the model Set and Save Views Create simple Rounds along model edges using direct modeling Understand the Round Tool HOLES AND ROUNDS A variety of geometric shapes and constructions are accomplished automatically with Pro/E, including holes and rounds (Fig. 4.1). These features are called pick-and-place features, because they are created automatically from your input and then placed according to prompts by Pro/E. A hole can also be created using the Extrude Tool and removing material, but it must be sketched. In general, pick-and-place features are not sketched (except for the Sketched option when you are creating a complex hole shape, such as a non-standard countersink or counterbore). The Round Tool creates a fillet, or a round on an edge, that is a smooth transition with a circular profile between two adjacent surfaces. Holes The Hole Tool creates a variety of holes. Types of hole geometry include: Straight hole An extruded slot with a circular section Sketched hole A revolved feature defined by a sketched section Standard hole A revolved feature created with UNC, UNF, or ISO standards All straight holes are created with a constant diameter. A sketched hole is created by sketching a section for revolution and then placing the hole on the part [Fig. 4.2(a)]. Sketched holes are always blind and one-sided. Sketched holes must have a vertical centerline (axis of revolution), with at least one of the entities sketched normal to the axis centerline [Fig. 4.2(b)]. Pro/E aligns the normal entity with the placement plane. The remainder of the sketched feature is cut from the part, as with a revolved cut.
112 Figure 4.2(a) Sketched Holes (CADTRAIN, COAch for Pro/E) Rounds Figure 4.2(b) Hole Placement (CADTRAIN) Rounds (Fig. 4.3) are created at selected edges of the part. Tangent arcs are introduced as rounds between two adjacent surfaces of the solid model. There are cases in which rounds should be added early, but in general, wait until later in the design process to add the rounds. Introducing rounds into a complex design early in the project can cause a series of failures later. Two categories of rounds are available: simple and advanced. Much of the time, you will create simple rounds. These rounds smooth the hard edges between two adjacent surfaces. Figure 4.3 Rounds
114 Figure 4.6 Model Information shown in Browser Create the first protrusion, click: Extrude Tool Sketch Plane--- Plane: select FRONT datum from the model as the sketch plane Sketch Orientation--- Reference: select TOP datum from the model Orientation: Top (makes TOP datum face up) click Sketch button References dialog box opens Close Toggle the grid on Though it is not necessary for the sketching of this section, sometimes the grid spacing needs to be altered to a different size. Grid spacing defaults at 30 units (30 inches or 30 millimeters depending on the units selected). You can change the grid size at any point in the sketching process. Change the size of the grid spacing by choosing the following commands: Sketch from the menu bar Options Sketcher Preferences dialog box displays with Display tab active [Fig. 4.7(a)] click Constraints tab to see options [Fig. 4.7(b)] Parameters tab Grid Spacing Manual activate Equal Spacing Values X type 15 Enter [Fig. 4.7(c)] Notice that you can also change the number of digits displayed with this dialog instead of setting them in the config.pro settings. After the sketch is regenerated, the 15.00-inch grid zooms out of view beyond the 6.00-inch long part model. Change the grid X and Y spacing to.25. Use the values and dimensioning scheme provided in Figure 4.8. Only three dimensions are required for the first extrusion.
115 Figure 4.7(a) Display Tab Figure 4.7(b) Constraints Tab Figure 4.7(c) Parameters Tab Figure 4.8 Top View
Click: Create an arc by picking its center and endpoints click on the center and then on the first endpoint [Fig. 4.9(a)] click on the second endpoint [Fig. 4.9(b)] The completed arc will have its radius displayed (Fig. 4.10). Repeat the command and create a second arc (Fig. 4.11). Create 2 point lines Add the four lines to create a closed section (Fig. 4.12). (Create two lines MMB and then repeat). centerline (Fig. 4.12) 116 Create 2 point centerlines add a horizontal Create defining dimension Add the height dimension. The radius (weak) dimension for the first arc will automatically be removed. move the dimensions to appropriate ASME standard positions (Fig. 4.13) modify the dimensions to the design sizes: click window-in the sketch to capture all dimensions Modify the values of dimensions, geometry of splines, or text entities change the dimensions to the design values (Fig. 4.14) Arc s center Figure 4.9(a) Arc s Center and Endpoint Figure 4.9(b) Arc s Second Endpoint Figure 4.10 Completed Arc Figure 4.11 Second Arc
117 Figure 4.12 Add Lines and Centerline Figure 4.13 Add and Move Dimensions Figure 4.14 Modified Dimensions
Click: Continue Standard Orientation note the yellow direction arrow (you may need to zoom out to see the complete part) slide the handle until the dimension is approximately 2.00 (Fig. 4.15) double click on the value and input the design value 2.188 (or 2.1875) (Fig. 4.16 and Fig. 4.17) Enter Resumes the previously paused tool LMB to deselect 118 Figure 4.15 Slide the Handle Until the Value is Approximately 2.00 Figure 4.16 Front View
119 Figure 4.17 Modify Value Click: click on Protrusion in the Model Tree RMB Edit to show dimensions (Fig. 4.18) MMB File Delete Old Versions MMB Figure 4.18 Completed Extruded Protrusion The next features will be the cuts created to remove portions of the protrusion. The cuts will complete the primary features of the part. In general, leave holes and rounds as the final features of the part. A majority of holes are pickand-place features that are added to the model at a similar step, such as when they are drilled, reamed, or bored during actual manufacturing. In most cases, this means after most of the machining has been completed. Rounds are the very last features created. A good many model failures occur when a set of rounds is being created. Leaving them as the final features reduces the effort needed to resolve modeling problems.
Create the first cut, click: Extrude Tool from dashboard click Remove Material Options Symmetric Section dialog box displays, Sketch Plane--- Plane: select TOP datum from the model as the sketch plane RIGHT datum displays as default Sketch Orientation Reference (Fig. 4.19) Sketch view direction: Flip Sketch button 120 Figure 4.19 Cut References Click: Standard Orientation delete the RIGHT Reference click on the three surfaces shown in Figure 4.20 Close to accept the References Orient the sketching plane parallel to the screen Tools from menu bar Environment OK Toggle the grid off Create 2 point lines sketch the two lines (Fig. 4.21) MMB to end the line sequence reposition the default dimensions as necessary (Fig. 4.22) Figure 4.20 Adding Three Surfaces as References
121 Modify the values for the dimensions by double clicking on a dimension and typing a new value (Fig. 4.23) Standard Orientation Coordinate systems off slide one of the depth handles to 3.00 (Fig. 4.24) MMB (Fig. 4.25) MMB Figure 4.21 Sketch Two Lines from the References Figure 4.22 Repositioned Dimensions Figure 4.23 Modify Dimensions
122 Figure 4.24 Slide the Cut Depth Handles to 3.00 You can use drag handles on certain features to change their dimensions. As you dynamically drag the handles, the features get larger or smaller, depending upon the direction you drag. Figure 4.25 Completed Cut The second cut is similar to the first one. The sketching plane and primary reference will remain the same. Command sequences may not show, as many explanations, tool tips, or other descriptive information for tools and commands, which are now familiar. New tools, icons, and commands will have the tool description and tip provided. This practice will remain in effect for the remainder of the text.
Click: Extrude Tool Remove Material Options Use Previous Sketch click on the left edge surface shown in Figure 4.26 Close to accept the References sketch the three lines (Fig. 4.27) MMB to end the line sequence reposition the default dimensions as necessary (Fig. 4.28) modify the values for the three dimensions by double clicking on a dimension and typing a new value (Fig. 4.29) 123 Figure 4.26 References Figure 4.27 Sketch Three Lines Figure 4.28 Move Dimensions as Required
124 Figure 4.29 Edit Dimensions Click: Standard Orientation slide one of the depth handles to 3.00 [Fig. 4.30(a)] MMB [Fig. 4.30(b)] MMB Figure 4.30(a) Slide Depth Handles to 3.00 Figure 4.30(b) Completed Cut
Redefine the first cut and change the dimensioning scheme as per the design (Fig. 4.16). 125 Click on Cut id in the Model Tree (Fig. 4.31) RMB Edit Definition Sketch add the dimension Delete the unneeded dimension (Fig. 4.32) modify the new dimension (Fig. 4.33) OK (Fig. 4.34) Standard Orientation (Fig. 4.35) MMB Figure 4.31 Redefine the First Cut using Edit Definition Figure 4.32 Add the new Dimension and Delete the 1.125 Dimension
126 Figure 4.33 Modify the Dimension Figure 4.34 Redefined Cut Figure 4.35 Standard Orientation Trimetric View The next feature to be created is a hole. This pick-and-place (direct) feature does not require a sketch. Start by creating a datum axis through the cylindrical surface of the part. The top surface will be the second reference for the coaxial hole.
127 Spin your part to clearly see the cylindrical surface. Click: Datum Axis Tool pick on the cylindrical surface (Fig. 4.36) OK Hole Tool from the right tool bar (status displays- Loading Hole Charts) Figure 4.36 Creating a Datum Axis Since a datum axis was created prior to the Hole Tool being selected [the datum axis is still selected (highlighted)], Pro/E will assume that the hole is to be coaxial (Fig. 4.37). Figure 4.37 Coaxial Hole Displayed
128 From the dashboard, click: Drill to intersect with all surfaces Placement tab (Fig. 4.38) click in (No Items) box under- Secondary references: pick the top surface (Fig. 4.38) as the Secondary reference change the diameter to.8125 Enter (Fig. 4.39) Standard Orientation MMB Figure 4.38 Coaxial Figure 4.39 Completed Coaxial Hole
129 The second hole will be a non-standard counterbore hole. Instead of using the Hole command, we could also create this hole with a revolved cut. Sketched holes are really nothing more than revolved cuts. Orient the part as shown (Fig. 4.40) Hole Tool pick on the horizontal surface of the first cut and the hole will display with handles for; hole position, diameter adjustment, depth adjustment, and two reference handles for establishing the dimensioning scheme (Fig. 4.40) drag one handle to the right side surface and the other handle to the TOP datum plane (Fig. 4.41) click on the Placement tab on dashboard to see Secondary references 1. Pick somewhere on this surface 2. Drag handle to end surface on right side of part 3. Drag handle until the TOP Datum highlights Figure 4.40 Hole Tool Figure 4.41 Drag Handles to Secondary References
130 Click: Front click and hold the handle at the center of the hole [Fig. 4.42(a)] and move it about the surface [Fig. 4.42(b)] double click on the dimension from the holes center to the TOP datum plane and modify the value to 0.00 [Fig. 4.43(a)] Enter Standard Orientation [Fig. 4.43(b)] (Fig. 4.44) Figure 4.42(a) Drag the Circle about the Surface Figure 4.42(b) Dragging the Circle Figure 4.43(a) Hole Centered on TOP Datum Figure 4.43(b) Standard Orientation Figure 4.44 Selecting Sketched Option
Sketched holes and revolved cuts are created with a section sketch. The section must be closed, and have a vertical centerline. All entities must be on one side of that centerline. Always use diameter dimensions. There is no such thing as a radius hole or a radius shaft. The counterbore diameter is.875. The thru hole diameter is.5625 and a depth the same as the part (1.125). The depth of the counterbore is.250. 131 Click: Tools Environment Apply OK dynamic hole displays with reference dimensions (Fig. 4.45) Activates Sketcher to create section Toggle the grid on sketch a vertical centerline sketch six lines to describe half of the hole s shape [Fig. 4.46(a)] Create a diameter dimension by picking the centerline, then the edge to be dimensioned, and then the centerline a second time. Place the dimension by picking a position with the MMB [Fig. 4.46(b)]. Add a second diameter dimension [Fig. 4.46(c)] Modify the values of dimensions [Fig. 4.46(d)] Figure 4.45 Hole Placement Pick 1 st and 3 rd Pick 2 nd Figure 4.46(a) Centerline and Six Sketched Lines Figure 4.46(b) Diameter Dimension
132 Figure 4.46(c) Add Dimensions Figure 4.46(d) Modified Dimensions Click: Standard Orientation Coordinate Systems off rotate with MMB (Fig.4.47) double click on the distance to edge value and change to 1.75 (Fig.4.48) MMB (Fig.4.49) LMB to deselect Figure 4.47 Hole Figure 4.48 Modify Distance to Edge (1.75) Figure 4.49 Completed Sketched Hole
Click on the counterbore hole in the Model Tree RMB Info Feature Feature info: HOLE displays in the Browser (Fig.4.50) Take some time to view all the information available. Click on a Dimension ID in the Browser, the dimension will display on the model. click on the quick sash collapse the Browser MMB File Delete Old Versions MMB 133 to Slide Bar (for more information) Figure 4.50 FEATURE info: HOLE Both holes are now complete. In Lesson 18, you will detail this part in a drawing. If the counterbore were for a standard fastener, you could have created it with the Create standard hole option. This option allows the varying of the counterbore diameter and depth but does not permit the thru hole diameter to be altered for the screw shaft size.
134 To complete the part, a number of rounds need to be created. The first round is an edge round between the vertical and horizontal faces of the first cut. Before you start, create a user specified view and save it to be used later. Use MMB to orient your view similar to Figure 4.51 then, click: Reorient view Orientation dialog box displays click: Saved Views expands to show list Name- type ISORIGHT (Fig. 4.52) Save OK TOP Standard Orientation ISORIGHT Geometry [Fig. 4.53(b)] lower right corner of the graphics window [Fig. 4.53(a)] The Smart filter provides context-sensitive access to the most common types of selectable geometry in any given situation. In addition to the Smart filter setting, the selection filter can be set to limit the scope of selectable items to a specific type depending on the situation and need. Here we are setting the filter to Geometry. Figure 4.51 User Oriented View Figure 4.52 Orientation Dialog Figure 4.53(a) Selection Filter Smart Figure 4.53(b) Selection Filter Geometry
Pick on the edge between the horizontal and vertical surfaces of the part RMB Round Edges (Fig. 4.54) slide a drag handle until the radius is.50 [Fig. 4.55(a-b)] MMB (Fig. 4.56) 135 Figure 4.54 Pick the Edge then RMB Figure 4.55(a) Move the Drag Handles until the Radius is.50 Figure 4.55(b) Radius is.50 Figure 4.56 Completed Round
In general, consider these recommendations for creating rounds: Try to add rounds as late in the design as possible (but before machining features) Place all the rounds on a layer and then suppress that layer to speed up your working session To avoid creating children dependent on the round features, do not dimension to edges or tangent edges created by rounds 136 Click: Round Tool Datum planes off Datum axes off Datum points off Coordinate systems off (All is the default Selection Filter) type.125 for the radius value Enter hold down the Ctrl key and select the edges [Fig. 4.57(a-e)] Sets from the dashboard (Fig. 4.58) MMB (Fig. 4.59) MMB MMB File Delete Old Versions Figure 4.57(a) Datum Features Turned Off Figure 4.57(b) First Edge Selected Figure 4.57(c) Second Edge Selected Figure 4.57(d) Continue Selecting Edges
137 Figure 4.57(e) Selected Edges Figure 4.58 Sets Figure 4.59 Completed Part Lesson 4 is now complete; continue on to the lesson project.
Lesson 4 Project 138 Figure 4.60(a) Guide Bracket Guide Bracket Figure 4.60(b) Guide Bracket Bottom The Guide Bracket is a machined part that requires commands similar to the Breaker. Simple rounds and straight and sketched holes are part of the exercise. Create the part shown in Figures 4.60 through 4.65. At this stage in your understanding of Pro/E, you should be able to analyze the part and plan the steps and features required to model it. You must use the same dimensions and dimensioning scheme, but the choice and quantity of datum planes and the sequence of modeling features can be different. Figure 4.61 Guide Bracket Drawing
139 Figure 4.62 Guide Bracket Drawing, Top View Figure 4.63 Guide Bracket Drawing, Front View
140 Figure 4.64 Guide Bracket Drawing, Right Side View Figure 4.65 Guide Bracket Counterbore Holes