EGR 110 Engineering Graphics File: N110IL4 Inventor Lecture #4 Reading Assignment: Read the following in Parametric Modeling with Autodesk Inventor 2011 by Randy Shih: Chapter 3 – Grid and Snap Settings, Holes Chapter 4 – Chamfer and Fillet Chapter 10 – Revolved Features, Circular Patterns Lecture Outline: GRID and SNAP Intervals Setup (Chapter 3) AutoCAD users may be familiar with setting up grids and enabling the “snap to grid” feature. Snapping to a grid is possible, but is not recommended in Inventor. However, having a grid in the background might be useful for approximating the sizes of objects as they are drawn. SNAP and GRID options can be set in Inventor using Tools – Document Settings – Sketch. Note that the “Snap Spacing” actually sets the grid spacing. Try various settings. Try zooming in and out and note how the grid spacing changes. Note in the following screen capture: - 8 minor divisions for every major - Minor Grid Spacing = Snap Spacing * Grid Display = (0.125 in/snap)(2 snaps/minor grid) = 0.25 in/minor grid Be sure to letter your name neatly (between the guidelines provided) on all worksheets. 8 minors at 0.25 each1) Select face 3) Select edge for Reference 2 and then enter dimension (1.75) 2) Select edge for Reference 1 and then enter dimension (1.25) Page 2 Features in Inventor Inventor includes two types of geometric features: 1) Sketched features (including extrusions, revolutions, and sweeps) 2) Placed features (including holes, fillets, chamfers, and shells) So far we have only used a sketched feature (extrusion) to create solid models Holes (Chapter 3) Draw a simple solid block (extrude a rectangle) and switch to an isometric view. Select Hole from the Part Features Menu (or press H on the keyboard). Note the three arrows on the Hole dialog box above. These represent the first three steps in creating a hole. 1) Face – Select the face where the hole is to appear 2) Reference 1 – Select an edge on the object and specify how far from this edge the hole is to be located (a dimension box will appear after you select the edge). 3) Reference 2 – Select another edge on the object and specify how far from this edge the hole is to be located.Page 3 As shown to the right: - Change the Drill Size (diameter) - 0.75 shown - Change the Termination to Through All - Click OK. The resulting solid is shown below: Editing a Placed Feature - Note that Hole1 now appears in the Browser. Right click on Hole1 and select Edit Feature. - Try editing various features, including: - Changing the diameter of the hole - Changing the location of the hole - Adding threads to the hole - Making the hole countersunk or counterbored - Changing the Through All option to Distance and set the hole depth.Chamfer Round Fillet Original object with sharp corners: Fillet Chamfer Round Chamfer Fillet Page 4 Chamfer and Fillet (Chapter 4) Sharp edges on objects are often rounded off using curved edges or straight edges. Technically a rounded inside corner is called a fillet and a rounded outside corner is called a round, but both AutoCAD and Inventor create them both using the Fillet command. Chamfers and fillets can be added to both 2D sketches and to existing solid features. Note: If possible, add chamfers and fillets to a 2D sketch before extrusion. If they are added later to a solid (as a placed feature), they are often added as late as possible in the sequence of operations so that they do not interfere with other operations. Note that a machinist creating a part would be likely to add chamfers and fillets after creating other key features. It is often useful to think of creating parts in Inventor using a sequence of operations that might be logical in actually building the part in a machine shop. Example of a part with chamfers, rounds, and filletsPage 5 Threads Note that threads placed inside holes are bit-map images added for appearance only (although the thread sizes used can be referred to when dimensioning). Threads do not appear on isometrics in drawing files; however, the threads are properly represented in other views. External threads – External threads can be applied using the Thread command from the part feature menu. Try creating the following object. Note the sequence of operations used as shown in the browser.Page 6 Revolution (Chapter 10) Another type of sketched feature in Inventor is a revolution. Revolutions are useful for features that are symmetrical about an axis. A revolved feature is formed by revolving a 2D sketch about a specified axis. Example: Creating a wheel using revolution Profile and axis Revolution dialogue box Revolved Feature of revolution Example: Creating the following revolved feature. Symmetrical Features (Chapter 10) Symmetrical Features can be added using the Circular Pattern or Rectangular Pattern command in Inventor (similar to the Array command in AutoCAD). Example: Suppose that we wanted to add 6 equally spaced threaded holes to the wheel created earlier.Page 7 1) Add a Sketch Plane to the side of the wheel. Select Project Geometry and pick the existing circular features of the wheel to project them onto the sketch plane so that points on those features can be easily accessed. Draw a construction line or use some other technique to locate the center point for one of the holes. 2) Finish the sketch and select Hole from the Parts Features menu. Use the following options: - Placement: From Sketch - Pick the center point for the hole - Termination: Through All - Threaded Hole – Select OK 3) Switch to an Isometric View to see the threaded hole just added. 4) Select Circular Pattern from the Parts Features panel. Then select: - Features: Select the threaded hole - Rotation Axis: Select the center holePage 8 Centerlines and Diametric Dimensions For revolved features it is often convenient to express diametric linear dimensions instead of radial dimensions. An example of the difference is shown below. Example using radial dimensions Example using diametric linear dimensions Revolved Features with Diametric Dimensions An example is used below to illustrate the procedure for creating a revolved feature using a centerline and diametric dimensions. 1) Draw the profile to be revolved. 2) Pick the centerline tool on the standard toolbar and then draw a line to create the centerline.