Spotlight on Features: Striving towards more intelligent feature patterns

In SOLIDWORKS 2015 we have added a new and more intelligent way to create linear patterns. This pattern uses existing geometry as reference and adapt to those circumstances.

Option 1: Up to Reference with fixed number of feature pattern instances.

Assume you have the following part (Fig. 1)

and want to create a four instances feature pattern in which the last instance is 100 mm from the end of the part as measured to the center of the feature (Fig. 2.)

As shown in (Fig. 3), you must select the “Up to reference” option and then select the end point reference vertex. Enter 100 mm distance to this reference point, and select the centroid option.

Option 2: Up to reference with feature instance separation gap

This is a variation of the above in that instead of having four instances feature pattern, now you need an X number of instances with a 50 mm gap between instances (Fig. 4.) Also, you want to have at least 150 mm gap at the end (reference point.)

To create this type of pattern you must select option “Up to reference”, select the part vertex reference point, select the gap between the feature centroid and the vertex (150 mm) and lastly select the gap between the features (50 mm.)

Option 3: Up to body and feature reference with gap feature distance

This variation uses a specific reference point in the seed feature as a gap to the body reference point.

You want to create a pattern with a 50 mm gap between features. You also want this pattern to end at least 100 mm before a specific point from the part and a feature reference (Fig.5)

To create this pattern you must first select the body reference point (Vertex1.) Then select the gap separation between this reference point and the feature reference point (Vertex2) (100 mm) and lastly either select the number of instances or the gap distance (50 mm) between each feature.

Mario Iocco

Mario Iocco

Sr. Technical Customer Support Engineer, SolidWorks, Americas.
Mario Iocco is a veteran CAD user. He started as a Mechanical Engineer first working in 2D with AutoCAD, moving on to 3D using  both SW and some  of the other CAD software on the market. He began his career with SolidWorks over 15 years ago. He started in R&D working on many of the new functionalities developed at the time -eDrawings, Sheet Metal, Weldments, etc. In the last few years, he moved to TS., working closely with VARs, Mario wrote the sheet metal functionality best practice manual, as well as creating hundreds of Sheet Metal Knowledge Base articles. He has presented webinars  on "Sheet Metal Tips and Tricks" and "Sheet Metal Bend Tables".