SolidWorks 2011 Parts Bible - Matt Lombard [140]
Vary Sketch allows the sketch of the patterned feature to maintain its parametric relations in each instance of the pattern. It is analogous to Geometry Pattern. Where Geometry Pattern disables the parametric end condition for a feature, Vary Sketch enables the parametric sketch relations for a pattern.
To activate the Vary Sketch option, the Linear Pattern must use a linear dimension for its Pattern Direction. The dimension must measure in the direction of the pattern, and adding the spacing for the pattern to the direction dimension must result in a valid feature.
The sketch relations must hold for the entire length of the pattern. Figure 9.14 shows the sketch relations and the resulting pattern. This feature does not have a preview function.
On the DVD
To better understand how this feature works, open the sample file from the DVD called Chapter 9 Vary Sketch.sldprt, and edit Sketch2.
Edit the .40-inch dimension. Double-click it and use the scroll arrow to increase the dimension; watch the effect on the sketch. If a sketch does not react to changes properly, then it cannot be used with the Vary Sketch option. In this case, the .40-inch dimension is used as the direction, because that is the dimension that will drive the sketch down the pattern. When using this option, the feature sketch must be driven by a single dimension. If the .48-inch dimension were anchored to the origin or the edge of the part like the .40-inch dimension, the pattern would not work properly. The direction dimension has to be able to drive the sketch in the same way that this one does. These dimensions cannot pass through the Zero value and cannot flip directions or move into negative values.
FIGURE 9.14
Using the Vary Sketch option
To make the sketch react this way to changes in the dimension, the slot was created using the bidirectional offset that was demonstrated in an earlier chapter, which means that the whole operation is being driven by the construction lines and arcs at the centerline of the slot. Sketch points along the model edges are kept at a certain distance from the ends of the slots using the .50-inch dimensions. The arcs are controlled by an Equal Radius relation and a single .58-inch radius dimension. The straight lines at the ends of the slots are controlled by an Equal Length relation.
This type of dimensioning and relation creation is really what parametric design is all about. The Vary Sketch option takes what is otherwise a static linear pattern and makes it react parametrically in a way that would otherwise require a lot of setup to create individual features. If you model everything with the level of care that you need to put into a Vary Sketch pattern feature sketch, then your models will react very well to change.
Using the Circular Pattern
The Circular Pattern feature requires a circular edge or sketch, a cylindrical face, a revolved face, a straight edge, an axis, or a temporary axis to act as the Pattern Axis of the pattern. All the other options are the same as the Linear Pattern — except that the Circular Pattern does not have a Direction 2 option and the Equal Spacing option works differently.
Equal Spacing takes the total angle and evenly divides the number of instances into that angle. The name equal spacing is a bit misleading because all Circular Patterns create equal spacing between the instances, but somehow everyone knows what they mean.
Without using the Equal Spacing option, the Angle setting represents the angular spacing between instances.
The Vary Sketch option is available in Circular Pattern as well. The principles for setup are the same, but you must select an angular dimension for the direction. The part shown in Figure 9.15 was created using this technique.
FIGURE 9.15
A Circular Pattern vary sketch
If you are creative with the sketch relations you apply to a sketch, you can get some pretty exotic results from patterns using the Vary Sketch option.