Chapter 1 AL Inventor Design Philosophy Create parametric designs •u Get the “feel” of Inventor •u Use the Inventor graphical interface •u Work with Inventor File Types •u Move from AutoCAD to Inventor •u Create 3D virtual prototypes •u Use functional design GH TE D •u MA TE RI In this chapter, you will be introduced to the concept of parametric 3D design and the general tools and interface of Inventor.
| Chapter 1 Inventor Design Philosophy You can see four dimensions placed on the two rectangles defining the length and width of each, along with a fifth dimension controlling the angle at which the two rectangles relate. These dimensions are parameters, and if you were to change one of them, at any point during the design or revision of the part, the sketch would update and adjust to the change.
Understanding Parametric Design the same part, and you can copy the part file to create variations of the original part. In order to assemble parts, you create geometric relationships called assembly constraints defining how the parts go together. The constraints are parameters that can be defined and revised by you at any time in the design process as well.
| Chapter 1 Inventor Design Philosophy shows every feature you create during the design of your part. Figure 1.5 shows the model browser for the pivot link file. Figure 1.5 The model browser showing the feature tree (history) of a part named Pivot_Link.ipt You can see that each feature is listed in the browser in the order it was created, forming a history tree. In order to create a part that handles changes predictably, you must create a solid foundation on which to build the rest of the model.
Understanding Parametric Design Driving Dimensions The workflow in Inventor sketching is substantially different from that of traditional AutoCAD, even beyond dimensions. In Inventor, you create sketches in 2D and then add geometric constraints such as horizontal, vertical, parallel, and so on to further define the sketch entities. Adding the geometric constraints allows line work to adjust in a predictable and desired manner and helps control the overall shape of the sketch.
| Chapter 1 Inventor Design Philosophy within the model, to achieve a complex design in the end. By creating a number of features within the model, you are able to independently change or modify a feature without rebuilding the entire model. An example of editing a feature would be changing a hole size. If you create a base feature first and then create a hole feature in that base feature, you can makes changes to both independently.
Understanding Parametric Design Assembly Modeling Best Practices Once you’ve created part files, you will put them together to build an assembly. And when you do, you want to build it to be as stable as possible, so that if you move, replace, or remove a part, the rest of the assembly will not fall apart. There are two parts to an assembly: links to the components it is made of and the geometric information about how those parts fit together.
| Chapter 1 Inventor Design Philosophy Router Base assembly is shown in the browser with a pushpin icon. This denotes that this assembly is grounded or pinned in place, and its coordinates cannot accidentally change. Keeping one grounded component in each assembly will allow you to fit other parts to it without it moving. You might imagine the old carnival game where you throw a ball at a pyramid stack of metal bottles. To win the game you had to knock down all of the bottles.
Understanding the “Feel” of Inventor Understanding the Intuitive Interface The overall interface of Inventor might be called context intuitive, meaning that it changes menus depending on task and environment. Inventor works by grouping tools onto tabs that offer only the tools needed for the appropriate task at hand. If you are sketching a base feature, the tools you see are sketch tools. In Figure 1.8 the 2D Sketch tab is active, and displayed are tools you use to create and dimension sketches. Figure 1.
| Chapter 1 Inventor Design Philosophy As you can see, the collection of tabs (called the Ribbon menu) changes intuitively with every task or environment you switch to. With a task-based user interface, there is no need to display every possible tool all at once. In the next section you will explore more of the user interface. Using General Tools vs. Specific Commands In this section you’ll compare the way Inventor tools are set up with those of AutoCAD.
Using the Inventor Graphic Interface | Using the Inventor Graphic Interface The Inventor graphic interface might be different from what you are accustomed to in other general software applications and even different from other design software. In Figure 1.12, you see the entire Inventor window, which shows an assembly file open for editing. Figure 1.
| Chapter 1 Inventor Design Philosophy Table 1.1 defines all the Quick Access toolbar icons available for the different file types. Table 1.1: Icon Quick Access toolbar icons Definition The New icon launches the New File dialog box. The drop-down list allows you to create a new part, assembly, drawing, or presentation file using the standard templates. The Open icon launches the Open dialog box. It displays a location defined in your active project. The Save icon saves the file.
Using the Inventor Graphic Interface Table 1.1: Icon Quick Access toolbar icons (continued) Definition The Design Doctor icon launches a dialog box that helps you diagnose and repair issues with a file. It is grayed out unless there is an issue. The Update All Sheets icon is used in the drawing environment to update all the sheets in a drawing at once. The Parameter icon is used to access the parameters table where you can rename, change, and create equations in dimension and design parameters.
| Chapter 1 Inventor Design Philosophy Exploring the View Cube The ViewCube, shown in Figure 1.15, is a 3D tool that allows you to rotate the view. Here are some viewing options: •u If you click a face, edge, or corner of the cube, the view rotates so the selection is perpendicular to the screen. •u If you click and drag an edge, the view rotates around the parallel axis. •u If you click and drag a corner, you can rotate the model freely.
Using the Inventor Graphic Interface | A Look at the Navigation Bar Continuing with the interface tour, you’ll see the navigation bar located on the right side of the graphics window. At the top of the bar is the steering wheel. Below the steering wheel are the other standard navigation tools: Pan, Zoom, Orbit, and Look At. Figure 1.16 shows the navigation bar. Figure 1.16 The Navigation Bar You can use the navigation bar’s steering wheel to zoom, pan, walk, and look around the graphics area.
| Chapter 1 Inventor Design Philosophy The Ribbon Menu The Ribbon menu is similar to the one introduced in Microsoft Office 2007 in that it is composed of tabs and panels. Each tab contains panels for a particular task, such as creating sketches, and each panel contains related buttons. As previously mentioned, the Ribbon will change to the proper tab based on the current task (for example, sketching brings up the Sketch tab), but you can select a different tab as needed.
Using the Inventor Graphic Interface | Figure 1.18 The View tab The Visibility panel has tools for controlling which objects are visible. When you click Object Visibility, a large list is displayed so you can control the appearance of your graphics window. The Appearance panel has tools for controlling the way models are displayed. You can switch between orthographic (parallel model lines appear parallel) and perspective (parallel model lines converge on a vanishing point) views.
| Chapter 1 Inventor Design Philosophy Using a perspective view may be desirable when viewing the model in a 3D view but can be distracting when sketching on a flat face or viewing the model from a standard 2D orthographic view, because you see what appears to be tapering faces and edges.
Using the Inventor Graphic Interface Using the Browser In this section, you will explore the behavior of the browser pane when working in Inventor by opening an assembly and making an edit to one of its parts: 1. Go to the Get Started tab, and click Open. 2. To ensure that you are looking at all the files in the Mastering Inventor 2011 project (and only the files in this project), click Workspace in the Open dialog box, as shown in Figure 1.19. Figure 1.
| Chapter 1 Inventor Design Philosophy When opening an assembly file, the Assemble tab of the Ribbon bar is active. You’ll notice that in the model browser (to the left of the screen) all items are shown in a white background, with no portion of the model browser grayed out. You are currently in the top level of the assembly, meaning that the uppermost level of the assembly is currently active and ready for edits. 4.
Using the Inventor Graphic Interface | Edit a Part Next you’ll continue with the exploration of the browser by setting a part file active for edits, and making a change to a part feature. 6. In the browser double-click the part called Face_Plate_mi_1 to set it active for edits. If you hover for a moment over the icon the plus sign may automatically expand, you can disregard that and just double click the icon.
| Chapter 1 Inventor Design Philosophy Four Ways to Use EOP Markers Since part features are listed sequentially in the order they were created, the EOP marker allows you to figure out how a part was constructed. Dragging the EOP marker to the top and then dragging it down one feature at a time recreates the part. This can be useful when working with parts designed by others and can be used as a powerful learning tool. You can use the EOP marker to insert a feature anywhere in the model tree.
Using the Inventor Graphic Interface | Return to the Assembly Now that your part feature is edited, you will leave the part level and return to the assembly level where you started out. 13. On the Model tab click the Return button on the far right. Notice that the faceplate is pulled back against the frame. This is the power of a parametric model.
| Chapter 1 Inventor Design Philosophy Figure 1.23 The Inventor Style And Standard Editor (assembly mode) 4. Close the Style and Standard Editor dialog box and then click the small X icon located just above the View Cube to close the assembly file. Note that there is an X at the very top right of the screen that closes Inventor completely; if you accidentally select that one simply restart Inventor and continue to the next step. 5. From the Get Started tab, click the New button. 6.
Learning the File Types in Inventor | Because the task of creating a surface extrusion is different than creating a solid extrusion some options are simply grayed out and not available. You will notice this throughout Inventor as options are offered and suppressed depending upon the task at hand. You can close the drawing file you have open without saving changes and continue on to the next section. Learning the File Types in Inventor In AutoCAD, you might be used to having the .
| Chapter 1 Inventor Design Philosophy •u .dwg (AutoCAD): AutoCAD nonassociative drawing file - is used to convert an Inventor drawing file to a standard AutoCAD file •u .xls: Excel files that drive iParts, threads, and other data - is used to manage tabled data, linked or embedded in a part, assembly or drawing file Although this list may seem intimidating, once you become familiar with Inventor, having many different file types will be less of a concern.
Moving from AutoCAD to Inventor | dimensions and other entities can be added and will remain intact when the file is opened again in Inventor, but as a rule, objects must be edited in the application from which they were created. Creating DWG Files from Inventor Drawings Users of Inventor may often find that they are called upon to create native AutoCAD .dwg files from Inventor .idw files for use by customers or other people within the company. A user may create a .
| Chapter 1 Inventor Design Philosophy If your experience is like that of many others who made the transition from the drawing board to drawing lines in AutoCAD, it was difficult to say the least. At first you may have been frustrated with spending more time creating electronic drawings than it would have taken to produce the drawing with the board. However, a key reason for the acceptance of AutoCAD was the ability to make edits far more quickly than you could with eraser and paper.
3D models vs. 3D Virtual Prototypes | have individual parts. All these components are constrained in such a way that the fit and functionality of all parts and mechanisms can be visualized, tested, and proven before any parts are manufactured. Scrap and rework are minimized or eliminated if the design is fully completed and proven in Inventor before it ever reaches the shop floor.
| Chapter 1 Inventor Design Philosophy too have the ways we design. However, it is possible to use new design tools in the same manner we used the old tools if we are not careful. As companies moved from the drafting board to AutoCAD, many users continued to use AutoCAD in much the same way they used the board. Not reusing data in the form of blocks and block libraries and not employing block attributes to pack those blocks with intelligence are common examples of this.
Understanding Functional Design | The V-belts Generator An example of functional design and its benefit is the use of the Inventor’s V-belts Generator. Traditionally, to design a pulley system, you would lay out the pulleys in positions as required by the design and then choose a belt that met the design requirements and came as close as possible to fitting the pulley spacing. The result oftentimes is that no common belt size fits the pulley spacing.
| Chapter 1 Inventor Design Philosophy The Bolted Connection Generator The Bolted Connection Generator is one example of a functional design tool. It can create and insert a complete bolted connection all at once by sizing the bolt diameter and length, by selecting the right parts and holes, and by assembling all the components together. You can create templates for common fastener stacks that you might use every day, as well.
The Bottom Line | The Bottom Line Create Parametric Designs The power of parameter-based design comes from the quick and easy edits, where changing a parameter value drives a change through the design. In order to make changes easily, though, you need follow certain general rules, so that the changes update predictably. Master It You want to create a model of a base plate, a rectangular-shaped part with a series of holes, and rectangular cutouts.
