# Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated)

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1 Inventor (5) Module 2: 2-1 Module 2: Radial-Line Sheet-Metal 3D Modeling and 2D Pattern Development: Right Cone (Regular, Frustum, and Truncated) In this tutorial, we will learn how to build a 3D model of a sheet metal part wrapping a right cone (regular, frustum and truncated), which is a solid of revolution, and which flat pattern is one of the two types of radial-line development (one in which element lines radiate from a common point called the vertex); we will accomplish this task with the Revolve and Extrude tools, which are generic 3D modeling tools from Inventor s Features panel. The basic procedures to complete this job in Inventor are to first draw a cut-off section profile of a regular or frustum of a cone (as shown in Figure 2-1C); and to use the Revolve tool to revolve this profile around an axis line into a 3D solid, with (instead of 360 since there needs to be a gap for Inventor to flat the pattern out). To cut the regular cone into a truncated cone, a profile that includes an angled line is drawn and used to cut the regular cone. After the truncated cone is created, we will move to Module 4: Intersection and Development of Sheet Metal Parts in Inventor, which introduces the topic of intersection and development of conic and other sheet metal parts, with the same tools previously learned but used in different ways. In addition, we will study how to use the Work Plane tool to solve important descriptive geometry problems in Inventor. Section 1: Creating the Sheet Metal Part Wrapping A Regular Cone Launch Inventor, start a new Sheet Metal (in).ipt file under English tab. Turn Visibility on for XZ and XY Planes, plus the Center Point from the Model panel. Sketch1 is created by default in the XY Plane (the one parallel to your computer s screen). Go to View Isometric for better visualization in 3D space; and click the Look At tool button to return to orthographic view and start creating the cross-sectional profile of the cone. For a frustum of a cone (one with the top cut off with a plane parallel to the base plane, or in this case, horizontally ), use the Project Geometry tool to project the Center Point for a snap first; then use the Line tool to draw a slanted line of the cross-section profile, plus a line of revolution staring from the projected Center Point (go to the Style

2 Inventor (5) Module 2: 2-2 pull-down menu to change the Style of the line of revolution to Centerline); then use the Offset tool to draw another slanted line parallel to the first one; use the General Dimensions tool to apply a Aligned Dimension between the two slanted lines; then use the Line tool again to draw two short line segments between the upper and lower endpoints of the slanted lines, so as to complete the profile, as shown in Figure 2-1A, make sure that the parallel lines representing the inside and outside walls of the conic sheet metal part are parallel, and connected with a short edge line perpendicular to both. Figure 2-1A: Profile sketch (left) and 3D solid feature of a frustum of cone (right) Figure 2-1B: Center Point, vertical line of axis, horizontal line, and angled line (Left); applying dimensions (middle); a gap at the vertex (right). For a regular cone (one with the vertex intact) that will be used to create a truncated cone later, we need a profile as shown in Figure 2-1B. Notice that not only the parallel lines representing the inside and outside walls of the conic sheet metal part are parallel; but also there needs to be a gap at the vertex of the cone, approximately the same size as the thickness of the sheet metal material (in this case, inch); or half of this (0.060 inch) from the line of axis of revolution. Use the Project Geometry tool to project

3 Inventor (5) Module 2: 2-3 the Center Point onto the sketch first; then use the Line tool to draw the vertical line of axis of revolution starting from the projected Center Point, and change the line Style to Centerline; then draw another vertical line next to the axis of revolution (in this case, to the right of it; and we called this line gap line ); then use he General Dimensions tool to apply a φ0.120-inch diametrical dimension as shown in Figure 2-1B (right); next, use the Line tool to draw a horizontal line starting from the projected Center Point with the help of snap, and an angled line (for the conic wall) starting at the endpoint of the horizontal line passing the ; then use the General Dimension tool to apply a 30 angular dimension between the angled line and the axis of revolution, and 12-inch linear dimension to the horizontal line. Next, use the Trim tool to trim off the segment of the angled line beyond the gap line (Figure 2-1B). Next, use the Offset and General Dimension tools to draw the second conic wall line parallel to the first one; then use the General Dimension tool to apply an Offset distance value of (same as the sheet metal material thickness); next, use the Line tool to draw two short line segments connecting the upper and lower endpoints of the slanted conical wall line and complete the profile (Figure 2-1C). Click the Return button to exit the Sketch mode. Create a folder named Tut 2-Cone and Intersection, in a convenient directory, save the file as Tut 3-Truncated Cone.ipt inside this folder. Save often. Figure 2-1C: Inside wall profile line (left); offset outside wall line (middle); completed section for regular cone (right). Click-select the Revolve tool icon from the Feature panel; the Revolve tool dialog window opens; in the Extents section, change from Full to Angle and type in the

4 Inventor (5) Module 2: 2-4 text field; click the Profile button and select the sectional profile; click he Axis button and select the axis line, green 3D geometry outlines appears on the screen; click the OK button (Figure 2-2A), and the 3D solid of the regular cone appears on the screen (See Figure 2-2B). Figure 2-2A: The Revolve tool window. Figure 2-2B: 3D solid of the regular cone. Section 2: Truncating the Regular Cone Click-select the XY Plane from the Model panel (or on the screen); click the Sketch button from the Command Bar; start to draw an angled truncating line and additional lines to make it a closed profile, with the help of the green snap indicator; then use the General Dimension tool to constrain the angled line to 30 with respect to the top horizontal line (Figure 2-3A). Next, use the Project Geometry tool and click-select the left edge of the 3D cone model; the edge line is projected onto the sketch. Next, use the Trim tool to trim off the top portion of the edge line above the truncating line (Figure 2-3B). Next, use the General Dimension tool to apply a linear dimension on the edge line for a height of 18-inch; the truncated edge line jumps up with the profile. Click the Return button to exit the sketch. Click-select the Extrude tool from the Features panel; in the tool window, choose Cut for Type, All for Extents, and Mid Plane for Direction, click the OK button to complete the truncated cone (Figure 2-3D). Save the file; and go to File Save A Copy As menu to save it as a new file as Tut 3-Truncated Cone Top.ipt, in the same Tut 2-Cone and Intersection folder. Close the current file.

5 Inventor (5) Module 2: 2-5 Figure 2-3A: Basic truncating profile before height is applied. Figure 2-3B Projected and trimmed edge line Figure 2-3C: Height dimension applied. Figure 2-3D: The truncated cone. Figure 2-4A: Clickselect the cone s truncated surface; and pick up the work plane Figure 2-4B: Click, hold and drag out a work plane. Figure 2-4C: Type in the Distance value. Figure 2-4D: Start a sketch on the new plane. Figure 2-4E: the projected outline, Center Point, and axis. Section 3: Creating the Top of The Truncated Cone We will create the top piece of the truncated cone in a way similar to what has been explained in Module 1A, but with a different approach on the creation of the profile

6 Inventor (5) Module 2: 2-6 sketch. The shape of the top appears to be an ellipse; however, due to the way the first 3D feature of the regular cone is created with instead of full 360, there is a gap in the edge outline of the truncated surface, making any projected profile sketch an open, not a closed path, which can not be used without some repair by the Sketch Doctor Examiner functions (Figure 2-4F), which is not always successful. We will try to avoid this problem, as will be explained in the following steps. Open the Tut 3-Truncated Cone Top.ipt file; and create a new work plane on the truncated surface of the cone. Click-select the truncated surface, then the Work Plane tool from the Sheet Metal (or Features, or Solid) panel; move the cursor closer to the surface; red outlines of the surface and a rectangular work plane outline appear (Figure 2-4A); hold down the mouse button and drag up any distance; a dimension text field appears (Figure 2-4B); highlight the value and type 0, click the green check mark (Figure 2-4C). The new work plane is created; rename the it Top Work Plane in the Model panel. Click-select the new plane; click the Sketch button; a new sketch screen appears (Figure 2-4CD). Use the Project Geometry tool, click on the edge outline of the truncated surface on the 3D model, and the Center Point feature in the Model panel. Draw one horizontal and one vertical axis lines, both starting from the projected Center Point and extending beyond the elliptical outline of the truncated surface, with the help of the green snap indicators (Figure 2-4E). Next, use the Trim tool to trim off the portion of the axis lines beyond the elliptical outline (Figure 2-4G). Delete the open projected elliptical outline. This provides three snap points for the new, closed ellipse (the Center Point, the major axis endpoint, and the minor axis endpoint, which are essential in the construction of an ellipse in any CAD program). Next, click-select the Ellipse tool from the Sketch panel; click on the projected Center Point, then one end point of one axis (major or minor); next, drag the curve out until it reaches the endpoint of another axis at click once at the appearance of the green snap indicator. The new ellipse is exactly the same as the outline of the truncated surface (Figure 2-4H); rename the sketch Top Face Sketch in the Model panel. A closed elliptical profile is now available (Figure 2-4I). Next, click-select all irrelevant features from the Model panel and press the Delete key on the keyboard to delete them, so that only the Top Work Plane and the Top Face Sketch remain (Figure 2-4J). Finally use the Face tool (with the Offset direction arrow upwards) to create the top piece (Figure 2-4K). The features of the 3D model are listed in the Model panel (Figure 2-4L). Save and close the file.

7 Inventor (5) Module 2: 2-7 Figure 2-4F: The Sketch Doctor Examiner. Figure 2-4G: Trim off the portion of the axis beyong the projected elliptical outline Figure 2-4H: Draw the new elliptical outline. Figure 2-4I: The closed outline. Figure 2-4J: Profile for the top piece. Figure 2-4K: The top piece. Figure 2-4L: The features listed in the Model panel. This completes the Modules 2. Congratulations! You have learned how to: Create the 3D models and flat patterns of sheet metal parts wrapping the volume of right-axis cones (regular, frustum and truncated.

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Chapter 4 Advance Dimensioning and Base Feature Options Learning Objectives After completing this chapter you will be able to: Dimension the sketch using the autodimension sketch tool. Dimension the sketch

### CREO.1 MODELING A BELT WHEEL

CREO.1 MODELING A BELT WHEEL Figure 1: A belt wheel modeled in this exercise. Learning Targets In this exercise you will learn: Using symmetry when sketching Using pattern to copy features Using RMB when

### AutoDesk Inventor: Creating Working Drawings

AutoDesk Inventor: Creating Working Drawings Inventor allows you to quickly and easily make quality working drawings from your 3D models. This tutorial will walk you through the steps in creating a working

### Bottom Rail. Chapter 2. Chair. A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. B. 3D Sketch.

Chapter 2 Chair Bottom Rail A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. Step 2. Right click Sketch on the Command Manager toolbar and select Weldments, Fig. 1. Step 3. Click

### Digital Camera Exercise

Commands Used New Part This lesson includes Sketching, Extruded Boss/Base, Extruded Cut, Fillet, Chamfer and Text. Click File, New on the standard toolbar. Select Part from the New SolidWorks Document

### < Then click on this icon on the vertical tool bar that pops up on the left side.

Pipe Cavity Tutorial Introduction The CADMAX Solid Master Tutorial is a great way to learn about the benefits of feature-based parametric solid modeling with CADMAX. We have assembled several typical parts

### Architecture 2012 Fundamentals

Autodesk Revit Architecture 2012 Fundamentals Supplemental Files SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Tutorial files on enclosed CD Visit

### When you complete this assignment you will:

Objjectiives When you complete this assignment you will: 1. sketch and dimension circles and arcs. 2. cut holes in the model using the cut feature of the extrusion command. 3. create Arcs using the trim

### MODELING AND DESIGN C H A P T E R F O U R

MODELING AND DESIGN C H A P T E R F O U R OBJECTIVES 1. Identify and specify basic geometric elements and primitive shapes. 2. Select a 2D profile that best describes the shape of an object. 3. Identify

### Working With Drawing Views-I

Chapter 12 Working With Drawing Views-I Learning Objectives After completing this chapter you will be able to: Generate standard three views. Generate Named Views. Generate Relative Views. Generate Predefined

### Applications in Technical Drawing

Applications in Technical Drawing Objectives: To use drawing aids in orthographic projection. To recognise the use of construction line in orthographic projection. To locate points using OSNAP and OTRACK.

Engineering Graphics ORTHOGRAPHIC PROJECTION People who work with drawings develop the ability to look at lines on paper or on a computer screen and "see" the shapes of the objects the lines represent.

ENGINEERING & COMPUTER GRAPHICS WORKBOOK Using SolidWorks 2005 Ronald E. Barr Thomas J. Krueger Theodore A. Aanstoos Davor Juricic SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com

### Tutorial Building the Nave Arcade

Tutorial: Digital Gothic AH C117B (Winter 2017) Tutorial Building the Nave Arcade Overview: Step 1: Determining and Drawing The Arch (Quinto Arch) Step 2: Extrude Molding Profile Step 3: Adding Walls Step

### Starting a New Drawing with a Title Block and Border

Starting a New Drawing with a Title Block and Border From the File menu select New. Within the New file menu toggle the option Drawing, name the file and turn Off the toggle Use Default Template. Select

### Chair. Bottom Rail. on the Command Manager. on the Weldments toolbar.

Chapter 2 Chair Bottom Rail A. Weldments Toolbar. Step 1. Click File Menu > New, click Part and OK. Step 2. Right click Sketch on the Command Manager toolbar and select Weldments, Fig. 1. Step 3. Click

New Sketch Editing/Adding 1. 2. 3. 4. 5. 6. 1. This button will bring the entire sketch to view in the window, which is the Default display. This is used to return to a view of the entire sketch after

### Engineering Technology

Engineering Technology Introduction to Parametric Modelling Engineering Technology 1 See Saw Exercise Part 1 Base Commands used New Part This lesson includes Sketching, Extruded Boss/Base, Hole Wizard,