- Coordinates for 3D CAD Modeling
- Geometric Entities
- 4.1 Manually Bisecting a Line or Circular Arc
- 4.2 Drawing Tangents to Two Circles
- 4.3 Drawing an Arc Tangent to a Line or Arc and Through a Point
- 4.4 Bisecting an Angle
- 4.5 Drawing a Line through a Point and Parallel to a Line
- 4.6 Drawing a Triangle with Sides Given
- 4.7 Drawing a Right Triangle with Hypotenuse and One Side Given
- 4.8 Laying Out an Angle
- 4.9 Drawing an Equilateral Triangle
- 4.10 Polygons
- 4.11 Drawing a Regular Pentagon
- 4.12 Drawing a Hexagon
- 4.13 Ellipses
- 4.14 Spline Curves
- 4.15 Geometric Relationships
- 4.16 Solid Primitives
- 4.17 Recognizing Symmetry
- 4.18 Extruded Forms
- 4.19 Revolved Forms
- 4.20 Irregular Surfaces
- 4.21 User Coordinate Systems
- 4.22 Transformations
- Key Words
- Chapter Summary
- Skills Summary
- Review Questions
- Chapter Exercises
This chapter is from the book
This chapter is from the book
This chapter is from the book
4.22 Transformations
A 3D CAD package uses the default Cartesian coordinate system to store information about the model. One way it may be stored is as a matrix (rows and columns of numbers) representing the vertices of the object. Once the object is defined, the software uses mathematical methods to transform the matrix (and the object) in various ways. There are two basic kinds of transformations: those that transform the model itself (called geometric transformations) and those that merely change the view of the model (called viewing transformations).
Geometric Transformations
The model stored in the computer is changed using three basic transformations (or changes): moving (sometimes called translation), rotating, and scaling. When you select a CAD command that uses one of these transformations, the CAD data stored in your model are converted mathematically to produce the result. Commands such as Move (or Translate), Rotate, and Scale transform the object on the coordinate system and change the coordinates stored in the 3D model database.
Figure 4.78 shows a part after translation. The model was moved over 2 units in the X-direction and 3 units in the Y-direction. The corner of the object is no longer located at the origin of the coordinate system.
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4.78 Translation. This model has been moved 2 units in the X-direction and 3 units in the Y-direction.
Figure 4.79 illustrates the effect of rotation. The rotated object is situated at a different location in the coordinate system. Figure 4.80 shows the effect of scaling. The scaled object is larger dimensionally than the previous object.
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4.79 Rotation. This model has been rotated in the X-Y plane.
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4.80 Scaling. This model has been scaled to 1.5 times its previous size.
Viewing Transformations
A viewing transformation does not change the coordinate system or the location of the model on the coordinate system; it simply changes your view of the model. The model’s vertices are stored in the computer at the same coordinate locations no matter the direction from which the model is viewed on the monitor (Figure 4.81).
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4.81 Changing the View. Note that the location of the model relative to the coordinate axes does not change in any of the different views. Changing the view does not transform the model itself.
Although the model’s coordinates do not change when the view does, the software does mathematically transform the model database to produce the new appearance of the model on the screen. This viewing transformation is stored as a separate part of the model file (or a separate file) and does not affect the coordinates of the stored model. Viewing transformations change the view on the screen but do not change the model relative to the coordinate system.
Common viewing transformations are illustrated in Figure 4.82. Panning moves the location of the view on the screen. If the monitor were a hole through which you were viewing a piece of paper, panning would be analogous to sliding the piece of paper to expose a different portion of it through the hole. Zooming enlarges or reduces the view of the objects and operates similar to a telephoto lens on a camera. A view rotation is actually a change of viewpoint; the object appears to be rotated, but it is your point of view that is changing. The object itself remains in the same location on the coordinate system.
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4.82 Common View Transformations. Panning moved the view of the objects in (a) to expose a different portion of the part in (b). In (c), the view is enlarged to show more detail. In (d), the view is rotated to a different line of sight. In each case, the viewing transformation applies to all the objects in the view and does not affect the location of the objects on the coordinate system. (Notice that the position relative to the coordinate system icon does not change.)
Viewing controls transform only the viewing transformation file, changing just your view. Commands to scale the object on the coordinate system transform the object’s coordinates in the database.
Examine the six models and their coordinates in Figure 4.83. Which are views that look different because of changes in viewing controls? Which look different because the objects were rotated, moved, or scaled on the coordinate system?
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4.83 Geometric or Viewing Transformation? Three of these models are the same, but the viewing location, zoom, or rotation has changed. Three have been transformed to different locations on the coordinate system.
You will use the basic geometric shapes and concepts outlined in this chapter to build CAD models and create accurate freehand sketches. The ability to visualize geometric entities on the Cartesian coordinate system will help you manipulate the coordinate system when modeling in CAD.
Industry Case: The Geometry of 3D Modeling: Use the Symmetry
Strategix ID used magnets to create a clean, quiet, zero maintenance brake for the exercise bike it designed for Park City Entertainment. When copper rings on the bike’s iron flywheel spin past four rare-earth magnets, they create current in circular flow (an eddy current) that sets up a magnetic field.
This opposing magnetic field dissipates power and slows the wheel. Moving the magnets onto and off the copper rings varies the amount of resistance delivered. When Marty Albini, Senior Mechanical Engineer, modeled the plastic magnet carrier for the brake, he started with the magnets and their behavior as the carrier moved them onto and off the copper rings (see Figure 4.84). “There is no one way to think about modeling a part,” Albini said. “The key is to design for the use of the part and the process that will be used to manufacture it.” To make the magnet carrier symmetrical, Albini started by modeling half of it.
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4.84 Flywheel Assembly. The magnet carrier for the brake was designed to move onto and off the conductor ring by sliding along an elliptical guide tube, pulled by a cable attached to the small tab in the middle of the carrier.
The magnet carrier was designed as a part in the larger flywheel assembly, parts of which were already completed.
Each pair of magnets was attached to a backing bar that kept them a fixed distance apart. To begin, Albini started with the geometry he was sure of: the diameter of the magnets, the space between them, and the geometry of the conductor ring. He sketched an arc sized to form a pocket around one of the magnets so that its center point would be located on the centerline of the conductor ring (see Figure 4.85). He then sketched another similar arc but with its center point positioned to match the distance between the centers of the two magnets. He connected the two arcs with parallel lines to complete the sketch of the inside of the carrier. This outline was offset to the outside by the thickness of the wall of the holder. (Because this is an injection-molded plastic part, a uniform wall thickness was used throughout.) One final constraint was added to position the carrier against the rail on the elliptical tube along which it would slide: the outside of the inner arc is tangent to this rail. With the sketch geometry fully defined, Albini extruded the sketch up to the top of the guide tube and down to the running clearance from the copper ring.
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4.85 Extruding the Carrier. The magnet carrier was extruded up and down from the sketch, shown here as an outline in the middle of the extruded part. Notice that the sketch is tangent to the guide tube rail, and the centers of the arcs in the sketch are located on the centerline of the conductor ring.
To add a lid to the holder, Albini used the SolidWorks Offset command to trace the outline of the holder. First, he clicked on the top of the holder to make its surface the active sketch plane. This is equivalent to changing the user coordinate system in other packages: it signals to SolidWorks that points picked from the screen lie on this plane. He then selected the top edges of the holder and used the Offset command with a 0 offset to “trace” the outline as a new sketch. To form the lid, he extruded the sketch up (in the positive Z-direction) the distance of the uniform wall thickness.
SolidWorks joined this lid to the magnet holder automatically because both features are in the same part and have surfaces that are coincident. This built-in operation is similar to a Boolean join in that the two shapes are combined to be one.
For the next feature, Albini created a “shelf” at the height of the rail on which the holder will slide. Using Offset again, he traced the outline of the holder on the sketch plane, then added parallel and perpendicular lines to sketch the outline of the bottom of the shelf. The outline was then extruded up by the wall thickness. The distance from the outside of the magnet holder to the edge of the shelf created a surface that would sit on the rail (see Figure 4.86).
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4.86 Changing the Sketch Plane. The surface of the rail was used as the sketch plane for the “shelf” on which the magnet carrier will slide.
Two walls were added by offsetting the edge of the shelf toward the magnet holder by the wall thickness, then offsetting the edge again by 0. Lines were added to connect the endpoints into an enclosed shape to be extruded. (In Solid-Works, an extrusion can be specified to extend in one or both directions, and to extend to a vertex, a known distance, the next surface, or the last surface encountered.) For the walls, Albini extruded them to the top surface of the magnet holder “lid.”
The connecting web between the magnet holders needed to match the shape of the elliptical tube in the flywheel assembly (see Figure 4.87). To make it, Albini sketched an ellipse on the newly created wall. An ellipse is a sketching primitive that can be specified by entering the length of the major and minor axes. Albini used the dimensions from the tube for the first ellipse sketch, then drew a second one with the same center point but with longer axes so that a gap equal to the wall thickness between them would be formed. The two ellipses were trimmed off at the bottom surface of the shelf and at the midpoint, and lines were drawn to make a closed outline. The finished sketch was extruded to the outside surface of the opposite wall.
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4.87 This view of the magnet carrier shows the elliptical shape of the connecting web and the rectangular shape of the tab. The parting line for the part, shown here as a dotted white line, is located at the edge of the fillet on the top of the magnet chambers.
More walls were sketched and extruded from the bottom surface of the shelf. Then, the wall over the connecting web was sketched and extruded down to the web.
The next step was to add the rounded edges for the top of the magnet holder. Albini invoked the Fillet command and selected to round all the edges of the top surface at once. As it created the fillet, SolidWorks maintained the relationship between the wall surfaces that intersected the top edge of the holder and extended them to the new location of the edge.
Next, Albini created a tab at the end of the part that would rest on the plastic collar in the assembly that went all the way around the magnet carrier. He first extruded a rectangular shape up from the top of the collar to form the “floor” of the tab. The walls of the tab required two additional extrusions.
The fillet at the top of the magnet holder provided the location for the parting line—the line where the two halves of the mold would come apart and release the part. Albini added a parting plane and used the built-in Draft option to add taper to the part so it would come out of the mold. After selecting all the surfaces below the parting plane, he specified a draft angle, and SolidWorks adjusted all the surfaces. This feature of SolidWorks makes it easy to add the draft angle after a part is finished. When draft is added, the geometry of the part becomes more complex and harder to work with. A cylinder with draft added becomes a truncated cone, for example, and the angles at which its edges intersect other edges vary along its length.
The next step was to add the bosses at the top of the magnet chambers that would support the bolts controlling the depth of the magnets. As it was a design goal to make the top of the chamber as stiff as possible to limit flex caused by the attraction of the magnets to the flywheel, the bosses were placed as far apart as possible, and ribs were added for rigidity. The bosses were sketched as circles on the top surface of the magnet holder with their centers concentric with the holes in the bar connecting the magnets below. Both bosses were extruded up in the same operation.
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4.88 Bosses and Ribs. Sketched circles were extruded to form the bosses on the top of the magnet chamber. The dotted lines shown here on the top of the chamber pass through the center point of the bosses and were used to locate the center rib and radial ribs.
Ribs in SolidWorks are built-in features. To create a rib, you simply draw a line and specify a width, and SolidWorks creates the rib and ends it at the first surface it encounters. To create the center rib, Albini sketched a line on the plane at the top of the bosses and specified a width (ribs on a plastic part are usually two thirds of the thickness of the walls). The rib was formed down to the top surface of the holder lid. For the ribs around the bosses, Albini did as Obi Wan Kenobi might have advised: “Use the symmetry, Luke.” He sketched the lines for ribs radially from the center points of the bosses (see Figure 4.88). To create the ribs, Albini created four of them on one boss, then mirrored them once to complete the set for one boss, then mirrored all the ribs from one boss to the other boss. Once all the ribs were formed, he cut the tops off the ribs and bosses to achieve the shape shown in Figure 4.89.
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4.89 This view of the magnet carrier shows the symmetry of the ribs and the shape that resulted from “slicing off” the top of the bosses after the ribs were formed.
The result was a stiffer rib and a shape that could not be achieved with a single rib operation. To complete the part, circles were drawn concentric to the bosses and extruded to form holes that go through the part (see Figure 4.90). Draft was added to the ribs and walls to make the part release from the mold easily. Fillets were added to round all the edges, reducing stresses and eliminating hot spots in the mold. Then, the part was mirrored to create the other half. The center rib and tab for attaching the cable were added and more edges filleted. Draft was added to the inside of the holder, and the part was complete.
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4.90 Circles concentric with the bosses were extruded to form the holes before the part was mirrored and remaining features added to finish the magnet carrier.
(Images courtesy of Marty Albini. This case study is provided as a courtesy by the owner of the intellectual property rights, Park City Entertainment. All rights reserved.)
CAD at Work: Defining Drawing Geometry
2D CAD programs may allow drawing geometry to be controlled through constraints or parametric definitions. AutoCAD is one software platform that now provides this tool. In AutoCAD, constraints are associations that can be applied to 2D geometry to restrict how the drawing behaves when a change is made.
Constraints are of two types:
Geometric constraints create geometric relationships between drawing objects, such as requiring that a circle remain tangent to a line, even when its radius is updated.
Dimensional constraints define distances, angles, and radii for drawing objects. These dimensional constraints typically can also be defined by equations, making them a powerful tool.
Usually, it is best to define the geometric constraints first and then apply dimensional constraints. This way the essential geometry of the shape is defined, and the dimensions can be changed as the size requirements vary.
Figure A shows an AutoCAD drawing that uses fixed and tangent constraints. The fixed constraint allows you to force a drawing object to stay in a permanent location on the coordinate system. The tangent constraint defines a relationship between two drawing objects, such as circles, arcs, and lines.
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(A) AutoCAD provides tools for defining geometric and dimensional constraints to control drawing geometry. (Autodesk screen shots reprinted courtesy of Autodesk, Inc.)
Understanding geometric relationships is a key skill for creating drawings that use parametric constraints. When geometric constraints are applied awkwardly or when the software does not provide a robust tool for constraining the shape, it can be difficult to get good results when updating drawings.