A Mechanical Desktop User's Look at Inventor

31 Jul, 2001 By: John E. Wilson

For the last year and a half Autodesk has had two programs—Mechanical Desktop and Autodesk Inventor—that essentially do the same sort of work and serve the same market. Both programs are feature-based parametric 3D solid modelers. Mechanical Desktop is the older program, and it has been, and probably still is, the most widely used program of its type. In spite of this, Autodesk has been intensively touting Inventor as the 3D modeler of choice for mechanical products and scarcely mentions Mechanical Desktop in its promotions and press releases. Nevertheless, Autodesk promises not only to continue supporting Mechanical Desktop, but to continue improving the program's capabilities. (Editor's note: Autodesk announced the release of Mechanical Destop R6 on May 15, 2001.)

Most of Autodesk's promotions for Inventor emphasize the programs ease of use without telling you anything about what Inventor's capabilities (and limitations) are, or even how the program works. Therefore, we'll take a look at Inventor in this months column. This will help Mechanical Desktop users understand the differences as well as the similarities of the two programs, and it also will help people who are not familiar with either program see what they can accomplish with Inventor.

Similar to Mechanical Desktop (and Solid Edge, SolidWorks, and even Pro/ENGINEER), Inventor is a feature-based, parametric 3D solid-modeling program. Feature-based means that models are constructed one feature, or component, at a time, while parametric means that the features are based on dimension values. Designs made by these programs are very flexible because you can change the size and shape of a model by simply changing dimension values. The programs are typically used for modeling items created by machining, molding, casting, forging, folding, and stamping processes.

Inventor File Types
Unlike Mechanical Desktop, in which a single file type is used in creating individual parts, assemblies of parts, exploded assemblies, and drawings, Inventor has four different types of files. Individual parts are created within files that have a filename extension of IPT. (A part is an item that is manufactured as one unit. A gear, a connecting rod, and a bolt are examples of a part.) When you model something composed of multiple parts, you will work within an assembly file, which has IAM as a file-name extension. Pictorial and exploded versions of assemblies are created in presentation files, which have IPN as a file-name extension. To create a 2D drawing of either a single part or an assembly of parts, you will work within a drawing file, which has a file-name extension of IDW.

We will concentrate on Inventor's tools for creating parts in this column because that is the most fundamental task of a 3D modeler. The real strength of Inventor, though, is in creating and managing assemblies that have many parts. Inventor has a system for grouping the part files of an assembly into projects, so that files are more readily shared among those who are working on a project and to help organize often-used as well as standard parts into libraries. Inventor can also create parts that adapt to differences in assemblies. You can create a spacer, for example, that will expand or compress as needed to fill the space between two parts in an assembly. You can also create adaptive subassemblies, design parts in place within an assembly, and modify existing parts to have them match the needs of an assembly.

Similar to Solid Edge and SolidWorks, Inventor has specialized tools for designing sheet-metal parts. These tools work in a special environment within part files in which such things as metal thickness and bend radii are set as operating parameters. We will discuss sheet-metal design in a future column, but for now we will just say that the process works well.

Inventor's Interface
Compared with Mechanical Desktop and other AutoCAD-based programs, Inventor has a relativity clean, simple appearance, as shown in Figure 1.

Figure 1. Compared with AutoCAD-based programs, Inventor has relatively few toolbars and pulldown menus. In part files, the browser shows all of the part's features in an outline-type format and shortcut menus that appear when you right-click a browser item. And when you right-click in the graphics area, you have access to most Inventor tools.
One reason for this simplicity is that Inventor does not have nearly the number of commands and operations that AutoCAD-based programs have. Inventor was built from the ground up for creating 3D models rather than 2D drawings, and, as a result, it does not have many of the specialized objects and operations—such as layers, polylines, stretching, multilines, leaders, and even dimensions and text—needed by AutoCAD. Inventor also does not contain operations based on old technology, such as AutoCAD's early attempts for setting viewpoint direction, or that are now handled by the operating system, such as tiled viewports.

Another reason for Inventor's clean screen is that, by default, it displays only those toolbars relevant to the current operation. For instance, when you are drawing a profile sketch, only the tools related to sketches are displayed. The pulldown menus at the top of the screen are also simplified. Unlike those of AutoCAD-based programs, menus for creating and editing objects are not included.

The Standard toolbar, located just below the pulldown menus, contains the basic Windows tools for file management, for view and visibility options, and for invoking help. Inventor does not have a Command line, but it does have a Command toolbar that displays messages and issues prompts. When you need to specify numerical data, such as a dimension value, a small dialog box will appear for you to use in entering the numbers.

As do virtually all parametric solid modelers, Inventor uses a browser to show part features in part files, the relationship between the parts in assembly files, and the relationship between views and sheets in drawing files. Context menus appear when you right-click items in the Browser, to give you a convenient alternate method for initiating many operations.

You can also initiate many operations from right-click context menus within the graphics area, as shown in Figure 1. And you can start some operations by pressing a key on your keyboard. The L key, for instance, starts the line tool, the D key starts the dimension tool, and F2 starts real-time pan.

Sketched Features
In all parametric solid modelers every part contains at least one feature based on a 2D sketch. The sketch can be drawn imprecisely because dimensions control the actual size of sketch objects, while geometric constraints control object orientation and relationships between objects. For example, you can constrain a line within a sketch to always be parallel to the x-axis, two adjacent lines to be perpendicular to each other, or two arcs to have the same radius. Sketch dimensions and constraints are the basis of the power and flexibility of parametric solid models, allowing you to change the size and shape of models by simply changing dimension values. Once a sketch is completed, it is either pushed perpendicularly (extruded), rotated about an axis (revolved), or pushed along a path (swept) to create a 3D solid feature. You can also use two or more sketches to make a solid through a process called lofting.

Sketches are always drawn on a sketch plane, which, in effect, is the xy plane of a movable coordinate system. A default sketch plane is always in place in a new file, so that you can immediately begin

Figure 2. Inventor solid models are based on 2D sketches similar to the one shown here. The orientation of sketch objects is controlled by geometric constraints, and their sizes are controlled by dimension values. This figure shows the constraint symbols for two of the sketch's objects. It also shows the small dialog box Inventor displays for you when entering or modifying dimension values.
drawing a sketch. Once a 3D feature exists, you can select an existing flat surface to serve as the sketch plane for another feature, as shown in Figure 2. If no suitable flat surface exists, you can create and position a work plane, and place the sketch plane on it. Ill explain more about work planes further on in this column.

Typically, a sketch represents the outline of the feature you intend to make. It must be completely closed, but you can supplement the outline with internal or external islands. Lines and arcs are by far the most common sketch objects, but you can use circles, ellipses, and even spline curves as sketch objects. Figure 2 also shows an Inventor sketch that is to be extruded to make a secondary 3D feature. Occasionally, you will need to include objects, which are called construction geometry, in the sketch to control geometry rather than to create geometry. Inventor has a special linetype for creating such objects.

Sketches are also used as paths for swept features. Inventor Release 4 introduced options for creating 3D sketches, which can be useful for creating sweep paths not confined to a plane. The tools for creating 3D sketches are somewhat primitive, but they are likely to improve with each future revision. Release 4 of Inventor can also create 3D surfaces, but here also the tools are primitive and limited.

Even though precisely drawn sketches are not necessary, and sometimes not even desirable, you can draw them precisely in Inventor. You can display a grid and you can snap to its nodes, and you can use a Precise Input dialog box to enter coordinate values in a variety of formats. As you draw sketch objects, symbols indicating geometric relationships with existing objects are displayed. For example, if the line you are drawing is perpendicular to an existing line, an upside down T appears next to both lines. The cursor automatically snaps to endpoints and centerpoints when it comes close to them. You can also perform a limited amount of sketch editing (trim and extend objects); create fillets, offsets, and copies; and rotate objects. To erase a sketch object, you pick a point on it to highlight it and then press the delete key.

By default, geometric constraints are automatically applied as you draw sketch objects. You can display the constraints with the Show Constraints tool. They are displayed as a row of symbols next to sketch objects, also shown in Figure 2. A tangent constraint, for example, is indicated by a circle that touches a slanted line; a horizontal constraint is indicated by a horizontal line over a horizontal base. You add constraints with the Create Constraint tool. Inventor has 10 different types of geometric constraints. Although Mechanical Desktop has 15 different constraints, the two programs are actually about equal in constraint ability because some Inventor constraints serve two purposes. For example, Inventor's vertical constraint accepts two points, and therefore can be used as an equal x coordinate constraint as well as forcing a line to be parallel with the y axis. Also, Inventor's coincident constraint acts much like Mechanical Desktop's project constraint.

Adding dimensions to Inventor sketches is intuitive and easy. After activating the dimension tool, you pick a point on an object and drag the cursor away from the object to establish the dimension text location. Inventor determines whether the object is a line, an arc, or a circle, and then it applies the appropriate dimension. You can also select two points in creating a linear dimension, and through a right-click context menu you can specify that the linear dimension is to be vertical, horizontal, or aligned. There is no parallel linear dimension as there is in Mechanical Desktop. Sketch dimensions are, in effect, symbols, similar to constraint symbols, and dimension values always face the front of the screen, regardless of the sketch's view direction. You can control the number of digits to the right of the decimal point, but you have no control over dimension color or arrowhead or text size and style.

The dimension tool is also used to edit dimension values. You pick a point on a dimension, and a small dialog box, also shown in Figure 2, appears for you to use in entering a new dimension value. As with Mechanical Desktop, each dimension has a name consisting of the letter d followed by a number assigned by the program. You can use these dimension names in formulas that set the value of other dimensions. And, you can assign formulas to dimensions directly or through a Parameters dialog box similar to Mechanical Desktop's Variables dialog box. You can also tie dimension parameters to an Excel spreadsheet file to create a set of dimensions that vary in order to fit particular design specifications for a part.

Placed Features and Work Features
Some features are based on existing geometry. They are referred to as placed features because they

Figure 3. This figure, which is a continuation of the model in Figure 2, shows a shell feature in progress. The faces shaded in green will be left open, while all of the others will become 0.125 inches thick. Previously Inventor's fillet tool was used to round all the model's sharp corners.
do not require sketches. Fillet features, for example, round the sharp edges of an existing feature. In using the fillet tool you specify the radius of the fillet and select the edges to be rounded. Shells are another useful type of placed feature in which the inside of an existing feature is scooped out to leave a relatively thin walled shell. Figure 3 shows a part that already has several fillet features and is about to be shelled to create an oil pan. Notice that a dialog box is displayed for you to use in setting the shell parameters and that you can exclude selected faces from the operation to leave openings in the part.

Hole features, which create drilled, counterbored, or countersunk holes, are an especially common type of placed feature. Inventor requires that the location of every hole be specified by a point

Figure 4. The model in Figure 3 has been shelled, and a profile for a flange has been drawn on a sketch plane placed on a work plane. The profile, which is shown in green, will be swept along the 3D path shown in red.
on a sketch plane. This is similar to the On Point option of Mechanical Desktop for locating holes. You can assign a specific depth to a hole, have it pass through all objects along its centerline, or terminate it when it reaches a selected face. The termination face can be curved. You can also create tapped holes in which threads are simulated by bitmapped images based on data in an Excel spreadsheet.

Similar to Mechanical Desktop, Inventor has work features used for the construction and control of other features. The points for holes mentioned in the previous paragraph are one example of a work feature. Work planes, which are used for positioning sketch planes and terminating extruded or swept features are another common work feature. Figure 4 shows a sketch on the work plane. In this figure, the sketch is about to be swept along a 3D path based on selected edges of existing features.

Figure 5. This is the completed Inventor model of an oil pan. The flange has been created, and holes have been made through it.
Figure 5 shows the same model after the sweep feature has been made, and after hole features have been added to the flange.

Although the steps to create and locate Inventor work features are similar to those in Mechanical Desktop, the properties and use of work features vary between the two programs. Work points and work axes, for instance, are recognized in Inventor only when they have been created on the current sketch plane, and they are not useful in connecting one feature with another.

The Bad and The Good
If you move from Mechanical Desktop to Inventor, you will find the two programs similar enough that you won't have much trouble adapting to Inventor's techniques for constructing models. However, they are dissimilar enough that you will have to change the way you perform many operations. Also, you are likely to find some of Inventor's features to be delightful while others are irritating.

Visibility is an area of Inventor that I have problems with. The program relies extensively on colors and icons, but you have very little control over color, and no control over the appearance and size of icons. For example, the general screen colors are restricted to eight different schemes, and you cant set the color of sketch objects, dimensions, and so forth individually. I have yet to find a color scheme in which all object types are easily seen in all circumstances. I also have problems with some of the icons, such as in distinguishing between the colinear and coincident constraint icons, and being able to even see the tiny icon used for work points.

Printed documentation supplied with Inventor consists of a 140-page Getting Started manual. This sparsely illustrated manual gives a good overall view of the program, but it does not tell you how to actually construct anything. The program depends on onscreen help, which is referred to as the Design Support System; however, the systems contents are mediocre. There is only superficial coverage of many major operations—lofting for example—and there are only a couple tutorials, none of which are for complex models.

I have no doubt that Inventor will eventually be Autodesks dominant, and possibly only, 3D modeler for mechanical products. Moreover, the need for a modeler not burdened with old baggage from the AutoCAD platform is obvious. You do not, however, need to be in a hurry to jump to Inventor, especially if you are currently a Mechanical Desktop user. At this stage in the development of each program, Mechanical Desktop has a slight edge in geometry creation abilities over Inventor. Furthermore, Inventor can import Mechanical Desktop part and assembly models and retain all of their parametric features. This means that you can continue to construct Mechanical Desktop models without worrying whether or not they will become worthless in the years ahead as parametric-modeling capabilities advance and programs consolidate.

About the Author: John E. Wilson

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