3 Ways to Design a Cone or Cylinder in SOLIDWORKS Sheet Metal

In this video, we’ll show you how to use the Insert Bends command to tackle three common use cases for designing and flattening a cone or rolled cylinder in SOLIDWORKS Sheet Metal.

Existing Hollow Cylinder

If we already have an existing hollow cylinder, we need to add a razor thin cut along the length of it so the part can be flattened. Lets begin by inserting a new sketch on one of the end faces of the cylinder. Sketch a rectangle and constrain the midpoint of the bottom edge to the center of the cylinder. Make the top edge tangent to the cylinder outside diameter. Next dimension the width of the rectangle to be a small number, something that is within your manufacturing tolerances. Use the Cut Extrude tool with the direction setting Through All.

Sketch a rectangle to insert cut in SOLIDWORKS

If the sheet metal tab is not visible on the command manager, right-click on any tab and select it. We can use the Insert Bends command to recognize this cylinder as a sheet metal part.

Insert bends command

Select one of the edges along the length of the cut to be the fixed edge. Now specify the desired K-factor or bend allowance. SOLIDWORKS automatically adds a sequence of features to designate the part as sheet metal to process the bends and create the flat pattern. Use the Flatten command to toggle between the flattened and rolled state.

How to make sheet metal parts easy in SOLIDWORKS >>

Design a Rolled Cylinder from Scratch

Now, let’s see how you might design a rolled cylinder from scratch. Start with a sketch. But instead of drawing a circle, use a center point arc. Sketch center lines from the origin to both open ends of the arc. Then dimension the angle to one degree. Extrude as a thin feature. Now use Insert Bends exactly like the previous example.

Designing a rolled cylinder from scratch

Rolled Conical Shape

A final use case is when you need a rolled conical shape. I’ll start by sketching the side view. First draw center line, then an angled line representing the outer edge of the cone. Add dimensions for the length outside diameter and inside diameter. Next, use the Boss Revolve tool to make a thin revolve feature, but set the angle to 359 degrees. Now I have a hollow cone with a razor thin cut. As before, this part is ready for the Insert Bends command. And below is the flat pattern.

Creating a flat pattern

It really doesn’t matter how you model a cone or cylinder, as long as the part has a thin cut along the length. It’s perfectly suited to be flattened using the Insert Bends command.

Learn more about Sheet Metal

Take a SOLIDWORKS Sheet Metal training course with Javelin live online to learn more advanced techniques.