The Revolve Features Unique Question

By John Landis on

The Revolved Boss and Revolved Cut features will sometimes prompt a message that isn’t found anywhere else in SOLIDWORKS.  You may have puzzled over this, wondering why you are even being asked this question and why only in a Revolve feature.

SOLIDWORKS warning pop up

This message pops up only when the sketch for Revolve features has these particular characteristics:

  • There is only one (1) open-profile entity or chain of entities in the sketch
  • The Axis of Revolution for the Revolve is a construction line

open profile axis

If the sketch has these attributes, you have seen this message when attempting to create a Revolve feature.  Answer “No,” and the feature creation proceeds as expected, i.e. the Thin Feature option is automatically selected because of the open-profile sketch.  Then specify the Thickness and end conditions and a thin-walled feature is created.

axis of revolve feature in solidworks

But if you answer “Yes” SOLIDWORKS does something interesting… In the sketch, it will automatically create a line entity that connects the endpoints of the open profile! It closes the profile and then proceeds with typical, non-Thin Feature creation.

non thin feature revolve

The preview still shows the centerline, but examining the sketch after creating the Revolved Boss reveals the added solid line entity.

revolved boss reveals solid line entity

You may think, “So what? Why is this question interrupting me? How often do I sketch an open profile when I really want a closed profile?” I have a theory why this function exists, and it ties back to another function commonly used with Revolved feature sketches, Dimension Doubling (DD).  DD is helpful because it allows us to think in and specify diameters when creating Smart Dimensions related to the Axis of Revolution.

The technique is simple; select a centerline and then some other solid sketch geometry. The dimension preview initially shows the distance between the entities. But if you then move your cursor to the other side of the selected centerline, the dimension doubles! Place the dimension text and then supply the parameter value. Again, this allows us to think and design in terms of the diameters rather than the radii of our Revolved feature. This technique can really streamline sketch definition and save time.

centerline reference

centerline reference

However, DD requires you to select a centerline as a reference.  So, often times we will convert a solid line Axis of Revolution to a centerline in the sketch to take advantage of DD.  We also often forget to convert the centerline back to a solid line before creating the feature.  I believe that is the reason for the, “The sketch is currently open…” message and question. I think the software developers realized that SOLIDWORKS users love DD but hate the disruption of changing the centerline back to solid, so they added this option to the workflow, so it happens automatically. What do you think of the Revolve features in SOLIDWORKS?