SolidWorks Toolbox has a tool for designing circular and linear cams, using a spreadsheet interface for data entry. You can access these and other design tools by turning on Toolbox (Tools> Add Ins> Toolbox). The circular cam tool makes a cam groove on the flat face.
There are many applications for circular cams with the groove on the cylindrical face. To make this these cams requires a different approach, using the Wrap feature (Insert>Features>Wrap). Start with a reference plane tangent to the cylindrical face and sketch the centerline of the cam groove. To make the groove wrap exactly around the cylinder, the horizontal length of the centerline must be (PI X Diameter).
Next, offset the sketch on both sides to set the width of the groove. “Select Chain” allows selection of one item in the path and have the selection include the entire path. “Bi-directional” offsets the sketch on both sides. “Make base construction” changes the original sketch to construction entities, and this is essential for the Wrap feature to work. Finally “Cap Ends” with the “Lines” option adds square ends to the offset sketch which will match each other when the sketch is wrapped.
The groove is created with the Wrap feature. Select “Deboss” to cut the sketch into the part, select the cylindrical face and enter the depth of the groove.