SolidWorks 2011 Parts Bible - Matt Lombard [52]
If you start an Equation Driven Curve in a 2D sketch, you get the form for a 2D curve equation. If you start in a 3D sketch, you get the form for a 3D curve. Once these splines are created, you cannot remove the relation to the equation and manually edit the spline; they are tied to the equation until you delete the entire spline.
One way to get around this limitation would be to create an equation-driven curve in one sketch, and then open another sketch and use convert entities to copy the spline, delete the On Edge relation, and use Simplify Spline to add control points to it. This is a technique commonly used with other types of curves; it does not enable you to update the overall size or shape of the spline through the equation, but you can manually adjust sections of a curve originally created from equations. Examples of where this might be useful would be a lead in or lead out on a cut thread, a special attachment loop in the middle of a spring, or a flare around the edge of a lens or reflector dish for mounting.
FIGURE 3.26
The Equation Driven Curve PropertyManager
Straight Slot and Curved Slot draw slots of a given width and length with full rounds on the ends. All the slot sketch entities can be seen in the PropertyManager shown in Figure 3.27. If you need to draw a composite slot or a slot with multiple entities, you will need to use the bi-directional sketch offset with capped ends mentioned earlier.
FIGURE 3.27
The PropertyManager for the slot sketch entities
Using the Dimensions/Relations toolbar
The Dimensions/Relations toolbar has a few tools that you have already seen, but as the name suggests, it also contains tools that will either help you to create or investigate dimensions and sketch relations. Figure 3.28 shows the default toolbar, but in the following pages, you look at all the available tools you can see at Tools⇒Customize⇒Commands⇒Dimensions/Relations.
FIGURE 3.28
The Dimensions/Relations toolbar
• Smart Dimension. Lets you dimension the sketch entity and combines several dimensioning methods into a single tool, such as horizontal, vertical, aligned, radial, diameter, and so on.
• Horizontal Dimension. Applies a dimension to a sketch entity that drives the horizontal distance between the endpoints.
• Vertical Dimension. Works like a horizontal dimension but vertically.
• Baseline Dimensions. Creates dimensions only in drawing documents. Baseline Dimensions are different from most of the dimension tools that you find on the Dimensions/Relations toolbar in that they can create driven dimensions on view geometry or driving dimensions on sketch geometry in a drawing, but cannot be used on sketch geometry in parts. Baseline Dimensions start from a single reference; then as you select additional references, additional dimensions are stacked (see Figure 3.29).
Figure 3.29
Baseline Dimensions on a drawing
• Ordinate Dimensions. Drives dimensions where a set of ordinate dimensions originate from a common zero point. To use these dimensions, simply click a zero location, place the zero dimension, and then click additional points. The dimensions are placed and are automatically aligned to the rest of the dimensions.
Note
If a line is not selected as the zero reference entity, the Ordinate Dimension feature defaults to a Horizontal Ordinate.
You can remove Ordinate Dimensions from the common alignment by right-clicking the dimension and selecting Break Alignment. Ordinate Dimensions will jog automatically if SolidWorks senses that the dimensions are getting too close to one another. You can also jog them manually. After you create the Ordinate Dimension set, you can add to it by accessing the Add to Ordinate command through the RMB menu. All the options for Ordinate Dimensions are shown in Figure 3.30.
Not all the listed options