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Manufacturing

Mechanical Desktop Features

31 Jan, 2000 By: John E. Wilson

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Autodesk's Mechanical Desktop incorporates both feature-based and parametric technologies in the construction of 3D solid models. Although these two terms sound very much like marketing buzzwords, they are not. They are vital components of the program. The feature-based technology enables you to build 3D solid models in a logical, step-by-step controlled manner; while the parametric technology enables you to establish relationships between features and to control the geometry of objects within them.

Features are the building blocks of Mechanical Desktop solid models. They are used for a wide variety of purposes, and they come in a wide variety of forms, ranging from a simple point to a complex 3D solid. Some features (such as work planes, round holes and fillets) are generated directly by Mechanical Desktop although they are based on user input. Other features (such as profile and 2D path sketches for making 3D solid features) are based on user-drawn objects. Some typical features are labeled on the 3D model shown in Figure 1.

Every feature of a model is listed in Mechanical Desktop's Browser in an outline-type format that indicates the order in which the features were created and how they are related. Figure 2 shows the Browser for the model shown in Figure 1. Notice that each feature has a name (such as Hole1 or ExtrusionBlind1) that is preceded by an icon, which is the same as the one on the toolbar button for creating the feature. You can also change the generic names that Mechanical Desktop assigns to features to more specific names such as No8screw Hole or Manifold_flange.

Figure 1. Mechanical Desktop incorporates both feature-based and parametric technology in constructing 3D models. Some of the features that this model is based on are indicated by the labels. Parametrics control the relationships between features, and because of them, the revolved feature in this model will remain on sweep feature if the sweep feature is changed.

Figure 2. Every feature of a Mechanical Desktop model is shown in the Desktop Browser is an outline type format that indicates the order in which the features were created and their relationship to each other. The browser in this figre is for the model shown in Figure 1.

Parametrics, on the other hand, control geometry, locations and sizes. In Figure 1, for example, parametrics enable you to easily change the length of the sweep feature. Moreover, the revolve feature will stay at the end of the sweep feature when you change the length of the sweep feature.

Although it is not apparent in Figure 1, each of the extrude, revolve and sweep features is based on a feature called a profile, and the geometry of each profile is controlled by parametrics. Also, the path that the profile for the sweep feature follows is controlled by a feature called a 2Dpath. Profiles and paths disappear when a 3D solid feature is created from them, but they continue to be listed in the browser (as shown in Figure 2), and they can easily be restored and edited.

Parametrics within a profile or 2Dpath are controlled by constraints. They come in two forms: geometric constraints and dimensional constraints. Geometric constraints (Mechanical Desktop sometimes refers to them as 2D constraints) control the geometry of a model. Through geometric constraints, for example, you can specify that two straight adjoining edges will always be perpendicular to each other, that a straight edge will always be tangent to an adjacent arc-shaped edge and so forth. Dimensional constraints control the size of objects. Although they look similar to ordinary AutoCAD dimensions, they actually determine the size of objects rather than simply report sizes. For instance, the diameter of a cylinder will be 23.5mm because that is the value you have assigned to its diameter dimension, and not because you drew the cylinder's profile to have a diameter of 23.5mm. If you later decide that the cylinder should be larger, you can simply specify a larger value for the diameter dimension, and the diameter of the cylinder will automatically increase.

As you construct 3D models in Mechanical Desktop, you will spend much of your time working with profiles and their constraints. Furthermore, correctly creating and constraining profiles is the key to constructing 3D models that are easily modified. So the rest of this column will concentrate on creating profile features. Since the application of constraints within profiles tends to be involved, we will save the discussion of them for a future column.

Sketched Features
Mechanical Desktop classifies profiles as a sketched feature. Altogether there are five different types of sketched features and five different commands for creating them, as shown in Table 1.

Table 1. Mechanical Desktop Sketch Types
Sketch Type	Command	Purpose
Profile	AMPROFILE	This command makes the profile of a 3D feature.
2D Path	AM2DPATH	This command makes a planar path for sweeping a profile when making a 3D feature
Splitline	AMSPLITLINE	This command splits faces of 3D features and splits a model into two separate parts.
Cutting Line	AMCUTLINE	This command makes an offset section view in a model that will be shown in a 2D drawing
Break Line	AMBREAKLINE	This command makes a breakout section within a model for a 2D drawing section view.

While these five sketch types serve different purposes and have different shape criteria, they are all based on ordinary AutoCAD objects, such as lines and arcs, that are drawn on a plane. They are referred to as sketches because you can draw them imprecisely and then use geometric and dimensional constraints to obtain the exact sizes and shapes you want. In fact, when drawing a sketch on the surface of an existing 3D feature, you will often deliberately draw it out of size and position so that you can more easily select objects and so that you can see the effects of the constraints and dimensions you add to the sketch.

It usually pays to be reasonably accurate when you draw sketches, though, to prevent them from becoming wildly distorted as you add geometric and dimensional constraints. For example, if you intend for an arc within a sketch to have a radius of 3 units, you should draw it so that its radius is in the neighborhood of 3 units even though Mechanical Desktop will force the arc to have the radius you specify when you add its dimensional constraint.

Profile Sketches
Profiles are the sketch type you will most often use, and they are the sketch type we will focus on in this column. Once you have created a profile sketch, you can use any of the following four methods to transform it into a 3D feature.

Extrusion is the process of making a 3D feature by pushing a profile perpendicularly from its plane.Rotation is the process of making a 3D feature by revolving a
profile about an axis.

Sweep lets you make a 3D feature by pushing a profile along a path. The path must have been made with either the AM2DPATH or AM3DPATH command. (See the Third Dimension column, "Smooth Sailing," CADENCE, December 1999, pp. 80-83, for a discussion of Mechanical Desktop's AM3D PATH command.)

Loft is when two or more profile sketches serve as cross sections of a 3D feature.

Profile sketches must be closed, but they do not have to be made from a single object. They can consist of any number of open objects that touch (or, because of constraints, almost touch) end-to-end. Valid AutoCAD wireframe objects for sketches include lines, circles, arcs, ellipses, splines and any member of the 2D-polyline family. You can also use edges of existing 3D features as sketch objects. Regions, 3D polylines, non-planar splines and self-intersecting objects (such as four lines that form a bow-tie figure) cannot be used in profiles.

Beginning with Mechanical Desktop Release 4, a profile sketch can contain multiple profiles or loops. When one loop is within another (larger) loop, the volume of the inside loop is subtracted from the volume of the outside loop when the 3D feature is created. When the

Figure 3. Mechanical Desktop now allows profile sketches to have multiple loops. As shown on the left in this figure, a loop within a loop removes volume from the 3D feature. As shown on the right, separated loops produce a disconnected 3D feature.

loops are separated, their volume is combined into one 3D feature even though there is empty space between the components of the feature. Figure 3 shows two examples of 3D features made from profile sketches that have multiple loops. Individual profile loops, however, cannot touch one another, overlap or be nested more than one level deep. Actually Mechanical Desktop will permit you to create sketch profiles in these configurations, but attempts to turn them into a 3D feature will fail.

Profiles with multiple loops are especially convenient when they are used with a 2D path to create a sweep feature. For example, a profile sketch consisting of a circle within a circle can be used with a sweep path to make a pipe fitting in one step. Otherwise, you must first create the outside diameter of the fitting by sweeping a circular profile along a path and then hollowing out the pipe by creating another circular profile and another sweep path that duplicates the first one.

However, profiles with multiple loops have significant limitations. One is that they cannot be used to create lofted 3D features, and another is that they cannot be used to create sweep features based on paths made from AM3DPATH's Pipe Path option. Furthermore, while sweep features based on paths made from AM3DPATH's Edge Path option can be made from multiple looped profiles, only one loop will be used in making the sweep feature. Also, the options for using planes to terminate extruded and revolved features are not available with profiles having multiple loops.

As a rule, any changes you make in a sketch's geometry will be done through constraints and dimensions rather than through AutoCAD editing operations. If, however, you need to change the number or the type of the sketch's objects such as to replace an arc with a straight line, you can erase AutoCAD objects in the sketch, draw new objects and incorporate the new objects in the sketch with the AMRSOLVESK command.

The Base Feature
Every Mechanical Desktop 3D model begins with a base feature. This base feature is a foundation to be built on and modified by dependent features in making a finished model. It is always based on a profile sketch. Drawing the profile sketch for the base feature

Figure 4. AutoCAD 2000 allows you to set different background colors for Model Space and Paper Space. This also allows you to control the background color of the plot preview, which is tied to the Paper Space background color.

is not only the first step in constructing a model, it has a great deal of control over how easily the model is made and how easily it can be modified. Therefore, it should have a form that will not cause problems if the model is modified. The base feature shown on the left in Figure 4, for example, is not a good one because it would be difficult to change the number of lobes or to make their thickness different from the center disk. A simple round disk is a much better base feature. You should consider the base feature as raw stock material that is to be carved, added to and supplemented by other features. Since all other features are dependent on the base feature, it cannot be deleted or even suppressed.

Sketch Planes
Sketches must be drawn on the current location of the Mechanical Desktop sketch plane. This plane is similar in these ways to the xy plane of AutoCAD's User Coordinate System (UCS):

It is a flat work area on which you can use your pointing device to draw objects.

It can be located anywhere in 3D space, and it can be oriented in any position.

The orientation of the x and y axes, along with the location of the origin, is indicated by AutoCAD's UCS icon.

Despite these similarities, the sketch plane is not the same as the UCS xy plane, and the two planes do not necessarily have the same location and orientation. When you move or reorient the sketch plane, the UCS xy plane automatically moves and reorients itself to match the sketch plane. However, the reverse is not true; the sketch plane does not move when you move the UCS xy plane.

The initial location of the sketch plane in Mechanical Desktop's template drawings is on the World Coordinate System xy plane, so you can often create the profile sketch for the base 3D feature without moving the sketch plane. Once you have created the base 3D feature, you will typically move the sketch plane to a flat face somewhere on it, create another profile sketch and 3D feature, move the sketch plane to a position suitable for a third 3D feature and so forth until your model is completed. Mechanical Desktop stores the sketch plane location and orientation for every sketch. Whenever you edit a sketch, its sketch plane is automatically restored.

The command that positions the sketch plane, AMSKPLN, is a little easier to use than AutoCAD's UCS command, but it is not as versatile. You will most often specify the sketch plane location by selecting an existing flat face, and you can do this by picking a point on the surface of the face or on an edge of the face. Then, you will specify the orientation of the x, y and z axes. Mechanical Desktop displays its animated cursor, along with an xyz-axes tripod, to help you orient the sketch plane. The animated cursor is an icon that looks somewhat like a rotating cylinder. The purpose of this icon is to simply signal that you can cycle through a list of command options by clicking the Pick button of your pointing device. The options available with AMSKPLN rotate the x and y axes 90 degrees. When those axes are in the directions you want, click the pointing device Enter button or the keyboard Enter key to set them and exit AMSKPLN.

You cannot specify the location of the origin of the sketch plane with most options of AMSKPLN. If you need to exactly position the origin of the sketch plane, you must first locate and orient the xy plane of the UCS and then use the UCS option of AMSKPLN to have the sketch plane match the current UCS xy plane. You will seldom need to do that, though, because you use constraints and dimensions to tie sketch objects to existing features rather than rely on coordinate points-the origin location of the sketch plane is generally not important.