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• Make Block. Creates a sketch block from selected sketch entities. You can position a manipulator to denote the insertion point for the block. Blocks may attach at any entity endpoint, but the insertion point follows the cursor.

• Edit Block. Enables you to edit an existing block as if it were a regular sketch.

• Insert Block. Enables you to select from a list of open blocks or browse to a location where blocks are stored. You can edit the insertion point by using the Edit Block function.

• Add/Remove. Enables you to add or remove sketch entities from the block without deleting them from the sketch while editing a block.

• Rebuild Block. Allows changes to a block to be reflected in any external relations without exiting the block. For example, if you have a block in a sketch and a sketch line is coincident to one of the endpoints in the block, you may edit the block such that the referenced endpoint moves. As a result, the line in the sketch will not move until you exit the block or use the Rebuild Block function.

• Save Block/Save Sketch As Block. Saves a selected block to an external file (with the *.sldblk extension) or saves the selected sketch as a block.

• Explode Block. Removes all the sketch entities from a block and brings them into the current sketch.

• Belt/Chain. Enables you to make a belt or chain around a set of pulleys. Each pulley must be a block. After activating the command (by right-clicking on a sketch or block), you can select each pulley and use the arrow on the pulley to switch the side of the pulley to which the belt goes. You can also compensate for the thickness of the belt (this is important when both sides of the belt are in contact with pulleys) and drive the pulley arrangement using the length of the belt. Figure 3.34 shows the Belt/Chain dialog box.

Figure 3.34

The Belt/Chain dialog box

Working with Reference Geometry

Reference geometry in SolidWorks is used to help establish locations for geometry that you can't physically touch, such as planes, axes, coordinate systems, and points. You often use reference geometry to establish a characteristic of the finished solid model before the model is created or to include an item that you may want to mate another part to in an assembly later. Mate References are also classified as Reference Geometry.

The importance of working with reference geometry becomes obvious in situations where you need to create geometry that doesn't line up with the standard planes. You might use planes to represent faces and axes to represent the centers of holes. Axes are often used to establish a direction, such as in plastic parts where, because of draft, you never truly have any vertical edges; an axis is frequently used to establish the direction of pull for the mold.

Coordinate systems come in handy, especially when translating a part from one system to another for the purpose of machining or some type of analysis. SolidWorks users usually model in such a way that the modeling work is made simpler by the choice of how the part origin is positioned relative to features of the part, but rapid prototyping, machining, mold building, and sheet metal manufacturing applications may have different requirements. As a part modeler, you cannot account for the needs of all downstream applications with your initial choice of origin placement, but you can always create a reference coordinate system for those downstream applications to use.

Creating planes

Planes are the most commonly used type of reference geometry because they are used for sketching, cutting, as extrude end conditions, and more. The Plane feature PropertyManager and its functionality have changed significantly in recent versions. With the new interface, shown in Figure 3.35, you start by selecting model items (faces, edges, points, vertices, or other sketch or reference geometry) that you want to use to create the plane. The new plane uses constraints like sketch relations from the selected references. For example, in Figure 3.35, the new