SOLIDWORKS Linear Pattern Feature with Vary Sketch Option

New for 2013 was an option for Linear and Circular Pattern
features that allow you to vary instances of your pattern with settings such as
dimension variances and spacing variances. 
But did you know that for many years now we have also had an option to
Vary the Sketch of the feature itself? 
In the Linear Pattern command found in part modeling, you have an option
to Vary Sketch when selecting a sketch dimension to follow for a
direction.  In the example below, I am
going to show you how to use this option by creating a ring of concentric,
equally spaced extruded rings as asked for by a recent student in one of our
CATI training classes.

Step 1, I made a circular boss extrude as feature #1 and
then created a new sketch on that top face and created a circle.  In this circle I used some different
dimension/relation techniques to use these as controlling items for the linear
pattern.  Notice the Sketch point with a
coincident relation to the outer edge of the circle, and the vertical relation to the origin of the center of
the circle.  Lastly, place the linear
dimension to use for controlling the size of the circle, as well as to control
the direction for the pattern soon to come.

Step 2, extrude this using a thin feature to control the wall
thickness.

Step 3, create a linear pattern of this thin extrude and use
the linear dimension as the direction 1 entity rather than a typical linear
edge.  Select the feature to pattern if
this wasn’t already selected and enable the Vary Sketch option.  Finally enter your dimension clearance between
rings and number of repeats.

And that completes the steps for this type of feature
pattern! 

Try it out yourself and see
what you can create with this old fashioned tried and true method.  Enjoy!

Brian Reel
Field Technical Services Manager

Computer Aided Technology, Inc.