Basics of the Sweep Feature in SOLIDWORKS

By Vince Farrell

If one just looks at the name “sweep feature”, it’s not readily apparent what this actually is. In my mind I hear “Sweep the leg!” from the first Karate Kid, which can’t possibly be correct. In all seriousness, when it comes to SOLIDWORKS,  the sweep is a powerful tool to create useful geometry when a regular boss won’t work. Using a sweep isn’t as confusing as it seems. The spoke of this wheel is an example of a swept boss/base:

I will be referring to the swept boss/base feature for this article, but the principles apply to a swept cut as well. The basics of a sweep are:

• Uses a minimum of 2 separate entities: a profile and a path; also, guide curves can be used to control the shape
• The path must intersect the plane of the profile

The “profile” is the shape that you want the outside of the sweep to have, and the “path” is what you want the profile to travel along/follow. In the spoke example, the profile and path sketches are identified and highlighted as blue and pink respectively:

Seems simple enough right? However...

In my experience, the first condition is pretty intuitive, but the second condition causes the most confusion. Here is an example of two sketches that won’t create a sweep because the path isn't intersecting the profile plane:

The simplest way to make sure both sketches intersect is to use the Pierce Relation. This relation makes a point pierce an axis, edge, or curve in another sketch, which is what we are looking for between the profile and the path of a sweep.

In this case, I've selected the endpoint of the vertical line and one of the construction lines from the center rectangle sketch:

Add the Pierce Relation and the endpoint and construction line touch:

By adding some more lines and a couple of fillets to Sketch2, my path sketch, we can make a shape that we couldn't do with an extruded boss/base and we’re ready to create the Swept Boss/Base:

Go to the Features tab of the Command Manager and click on the Swept Boss/Base to go into the feature.

If you have your two sketches selected already, SolidWorks should be able to auto-populate the Profile and Path field. If these aren't selected, you can click on these in the graphics area or from the Flyout Feature Manager Tree. The blue box is for the Profile and the pink box is for the Path:

Just hit the green check and you have a sweep!

If a twist is needed in the part, you don’t have to change the path to a helix (that might be a future blog article...) Within the sweep feature, under the Options area, the Orientation/twist type can be modified from Follow Path (the default) to Twist Along Path by hitting the drop down:

Select if the twist is defined by Degrees, Radians or Turns, put in the value of the twist and hit the green check:

For a video of the basic sweep feature, along with an introduction to Selection Sets, please take a look at our YouTube video below. Good luck sweeping and thanks for reading!