Points, Planes and Other Things

Despite marketing claims to the contrary, constructing parametric 3D models, such as those using Autodesk's Mechanical Desktop, is not at all like 2D drafting. It is not necessarily harder, but it is different. For one thing, much of the drafting and drawing needed to build a 3D model is done by the program itself. The saving in drawing time and effort, however, is offset by the need for the user to add controls and constraints to the objects that make up the model.

In addition to being the glue that hold things together, constraints control the size, shape and location of objects. Internally, most 3D features are controlled by geometric constraints and dimensions. Externally, they are often controlled by work features. We will take a look at Mechanical Desktop's work features in this article. We will see what they are, how they are created and what can be done with them. Three different work features exist, and they are created by three different Mechanical Desktop commands, as shown in Table 1. We will refer to just command names in this article, even though you are more likely to use a toolbar button or one of the several menus to create the feature than you are to type in a command name. We want to focus on how the commands work, rather than on how to start theM.

With one exception, work features are Mechanical Desktop-created objects, rather than user-drawn objects. You simply specify their location and, for work planes, their orientation. They are real objects, though, and they can be selected just as any line or 3D feature edge can be selected. In most cases, work features are parametric. That is, they are moved and reoriented as the feature they are attached to is moved, modified and reoriented. Mechanical Desktop puts them in the automatically created AM_WORK layer, and they show up in the Desktop Browser with names such as WorkAxis1 or WorkPlane3. If your model becomes too cluttered, you can individually turn their display off. You can also delete them, but do so with care, since features they are associated with may be deleted also.

Work Points
Work points are displayed as three mutually perpendicular lines that intersect at the work point. They are created by the AMWORKPT command, which will issue a command line prompt for the point's location on the current sketch plane. Typically, once the point is created, you will dimension or constrain it to existing features, such as path or profile sketches, existing 3D features and so forth.

A common use of work points is in making round holes (through the AMHOLE command) in curved or irregular surfaces, where there are no edges suitable for positioning the hole. Notice on the left-hand side in this figure how the work point is tied to the cylinder through dimensions. Even after the hole is made, you can restore these dimensions and change them to move the work point and, with it, the hole. You will also use a work point as the center of a polar array when the geometry is such that a work axis is not appropriate. Lastly, a work point can be used to tie a surfcut feature (made with the AMSURFCUT command) to existing 3D geometry. Then, as you move the work point, the surfcut feature will move with it.

Work Axes
Work axes are centerline-type objects extending along the axis of most 3D features that are geometrically capable of having an axis, such as a round hole, a cylinder, a partial cylinder or a torus. You can also draw your own work axis (this is the exception in creating work features we mentioned a few paragraphs ago). Once work axes have been created, they remain with the feature, regardless of how the feature is located or oriented. They are created by the AMWORKAXIS command, which will issue a command line prompt for you to either select an arc-shaped surface or a curved edge on a 3D feature or to sketch a work axis.

If you select an arc-shaped surface or edge, which is the default option, Mechanical Desktop will create the work axis for you, placing it collinear with the geometric axis of the 3D feature. You can select just one feature with each call to AMWORKAXIS. Often, you will use these work axes for constraining and dimensioning profile sketches. Although you cannot use a work axis to close a sketch, you can often tie the sketch to the work axis with a collinear geometric constraint. A work axis can also serve an axis of revolution for AMREVOLVE, as the center of a polar array and as an edge for positioning work planes.

The Sketch option of AMWORKAXIS allows you to draw your own work axis anywhere on the current sketch plane, just as if you were drawing a line. Often, though, you will use object snaps to tie the work axis to existing geometry. Sketched work axes can be used for the same purposes as placed work axes. In addition, you can position a work plane to be perpendicular to one end of a sketched work axis, and you can use a sketched work axis as the center of a 3D helix path sketch (made through the AM3DPATH command). In fact, if you want to create a 3D coil or spiral spring, you will probably base it on a sketched work axis, rather than on a cylindrical feature.

Work Planes
For the most part, parametric models are constructed on a plane-by-plane basis. You create a 3D feature from a 2D sketch, and then you move to another plane to create a 2D sketch for another 3D feature. Work planes can be a big help in moving to and setting up the next plane. When you are analyzing your model to see how you can set up the next plane, you will first look for planar faces that can be used to establish a sketch plane. If there is nothing suitable, you will then look for ways to establish a work plane on which you can locate a sketch plane. (This is a good place to emphasize that while work planes and sketch planes are both flat and have an infinite size, they are not the same. If you want to draw something on a work plane, you must place a sketch plane on it.)

Although your primary use of work planes will be to establish sketch planes, they are also useful for dimensioning and constraining sketches, for terminations of 3D features and for defining a cutting plane for full-section views of 3D parts in 2D drawings. Work planes are displayed as rectangles, which are automatically sized to fit the 3D model, and you can pick the edges of the rectangle for dimensions, constraints and object selections. However, since the displayed edge is not actually the boundary of the work plane, dimensions and constraints only work when they are perpendicular to the work plane.

You will virtually always create a work plane only when you have existing 3D features, and generally the work plane will be attached to existing 3D features. When you are positioning a work plane, it can be helpful to picture it as a large, rigid flat object, such as a sheet of plywood, that must be placed on, or attached to, objects in such a way that it is stable. Just as a sheet of plywood would not be stable if you laid it on just two sharp points, a work plane will not be stable if it is attached to just two points or vertexes. On the other hand, the plywood sheet would be stable if you laid it on two straight steel rods, and likewise, a work plane will be stable if it is attached to two straight edges or work axes (provided the two rods or two edges are in the same plane). Unlike a sheet of plywood, though, work planes are not affected by gravity. Also, Mechanical Desktop will not allow you to place a work plane in an unstable position.

Work planes are created through the AMWORKPLN command. This command uses a dialog box for you to specify the plane's position parameters, and it issues command line prompts for you to select objects for positioning the plane. The dialog box has two main clusters of radio buttons-one cluster is labeled 1st Modifier, and the other is labeled 2nd Modifier. These modifiers are similar to constraints in fixing the position of the work plane. Except for the Normal to Start, On UCS, World xy, World yz and World xz modifiers, no single modifier is sufficient to define a work plane's position. Attaching a work plane to an axis, for instance, will only partly fix the location of the plane, and you must specify a second modifier to prevent the plane from spinning about the axis. Usually, you will initially select a 1st Modifier. Then, the 2nd Modifiers that are not appropriate for use with the 1st Modifier will be grayed-out. A description of these modifiers is given in Table 2, and the allowable combinations of 1st and 2nd modifiers are shown in Table 3.

As an example of how the modifiers work, suppose you want to place a work plane on a curved surface so that it is perpendicular to an existing plane. You will select Tangent as the 1st Modifier and Planar Normal as the 2nd Modifier. After clicking the radio buttons for these two modifiers, you will press the OK button in the dialog box, and Mechanical Desktop will issue a command line prompt for you to pick a curved surface and another prompt for you to pick a plane. The new work plane will be placed on the curved surface, and it will be oriented to be perpendicular to the selected plane. In this example, as is often the case, you could just as well have used these two modifiers in the reverse order.

The On UCS, World xy, World yz and World xz modifiers, which are not described in Table 2, are only available by themselves-when any of them are selected, all of the 2nd Modifier buttons will be grayed-out. The On UCS modifier places the work plane on the User Coordinate System's xy plane, and the other three place the work plane on the stated plane of the World Coordinate System. They are referred to as non-parametric work planes because their relative position and orientation to the 3D part is fixed. The left side of this figure shows a dependent 3D feature that is based on a sketch located on a work plane that is on the WCS xz plane. The work plane, and consequently the sketch plane as well, is at an unchanging distance from the center of the cylinder. If you increase the diameter of the cylinder, the cylinder's surface will come closer to the flat face on the dependent feature, and the cylinder can eventually even engulf it.

These results will be exactly what you want if the distance from the center of the cylinder to the face of the dependent feature is important in the design of this part. On the other hand, if it is important that the face of the dependent feature remain a certain distance from the surface of the cylinder, you would probably place a work plane on the surface of the cylinder (using a Tangent modifier) and a second one, with the sketch plane, at the desired distance from the first one (using the Offset modifier).

While each of the non-parametric modifiers initially place the work plane on the stated plane, their relationship is with the part, rather than with the UCS or the WSC.

This finishes our look at Mechanical Desktop's work features. They are just one of the many new tools that have nothing to do with drafting that you must nevertheless learn to use if you are to be successful in making parametric solid models.