Creating a pattern of features / bodies along a curve is a very useful feature in SolidWorks. Previously, I discussed how to pattern features along a curve using Pro/Engineer, and the technique using SolidWorks is similar, but there are some differences in the work flow between the two CAD software packages.

First Body (SolidWorks)

Unlike Pro-E, creating the pattern in SW differs in the following:

• An anchoring surface or solid body is not required to create the pattern

• The first datum point does not necessarily need to be at the start of the curve (0, 0) in order for the pattern to continue to follow the curve.

Instead, the start point can be located some distance away from the end of the curve. However, for equal spacing in the pattern, the datum point should be at the start of the curve (0, 0).  To create the datum point, I recommend using the 3-D Sketch feature and creating a sketch point to use as the datum point. This provides more control than the point feature (Reference Geometry –> Point), which is not nearly as versatile as Pro-E’s datum point feature.

Before creating the sketch of the feature to be patterned, create a datum plane through the spline and point (3-D Sketch) and select the “Normal to Curve” option. The axis of revolution in the feature sketch will be aligned to this datum, and this is necessary to control orientation of the feature as it is patterned. While in Pro-E, a revolved feature could be created with the option of toggling between a solid or surface body, SolidWorks work flow dictates that the revolve feature must be selected under Boss/Base for a solid body revolve, and Surface for a surface Body revolve. There is no toggling back and forth in SolidWorks between the solid revolve and the surface revolve as these are different features.

Curve Driven Pattern Tool (SolidWorks)

To create the pattern along a curve, use the “Curve Driven Pattern” tool (Insert –> Pattern /Mirror –> Curve Driven Pattern). For the pattern direction, select the spline / curve, the number of instances, and the “equal spacing” option if equal spacing is desired (set datum point distance to 0, 0). The curve method option should be set to “Offset Curve”, and set the alignment method to “Tangent to Curve”.  As with Pro-E, SW permits pattern members to be skipped in the “Instances to Skip” option. To skip an instance, select the dot of the pattern instance. Select the dot again to restore the pattern member.

Note: “Bodies to Pattern” option was chosen instead of “Features to Pattern” option.

The revolved solid body cannot be merged with the surface body, and this requires the body instead of the feature to be selected for patterning.  If you wish to remove the first instance at the end of the curve, use the “Delete Bodies” tool (Insert –> Features –> Delete Body). To remove the surface for anchoring the pattern, the “Delete Body” tool can be used as well, and the pattern will appear to float in space.

Complete Pattern (SolidWorks)

It was noticed that the SW part files was approximately twice the size of the Pro-E part file. This could be due to different geometric modeling kernels, or the use of bodies instead of features for patterning in the part file. Both SolidWorks & Pro-E accomplished the task, so it is difficult to say which 3-D CAD software is better for creating a pattern along a curve as each has its own strengths and weaknesses.