Problem

This article goes over one of the frequent questions we get in support. How to model accurate swept cuts on a cylinder. Like all sweeps, the important elements are the path, profile, guide curves, and controlling options.

Solution

Use the following workflow for accurate tool-body cuts:

1. Open SOLIDWORKS and start by creating a simple cylinder with Boss Extrude

2. Create a simple 2D sketch that will get wrapped around the cylindrical face

   

3. Wrap the sketch (Insert > Features > Wrap) using the scribe option to create a split face that looks like an engraving. The key is to create a closed profile that only extends past one end of the cylinder.

   

4. Create a Ruled Surface (Insert > Surface > Ruled Surface) along one side of the outline using the Normal to Surface option.

   

5. Use Surface Extend (Insert > Surface > Extend) to extend the bottom edge of that ruled surface slightly (by .01” here) so that it intersects the cylindrical body. Being tangent is not enough for the next step.

   

6. Use Surface Offset (Insert > Surface > Surface Offset) to offset this surface .2" since the overall width of the slot is .4".

   

7. Now we have a surface body that intersects the centerline of the slot. We are going to use this surface body and the face of the slot to create a 3D Intersection Curve. Start a 3D sketch, select the surface body and the face, and use Intersection Curve (Tools > Sketch Tools > Intersection Curve).

   

8. We now have the path of the sweep, and we can create the profile for the sweep with a 2D sketch on the bottom of the cylinder.

   

9. Create a Sweep (not a Swept Cut) using the 2D Profile sketch and the 3D Path sketch, and for the guide curves, use the left and right edges of the slot created by the original Wrap feature. A couple of important notes about the Sweep. We are using a Swept Boss because we do not want to remove material yet. Also, we want to make sure we have the options set to Follow Path and 1st Guide Curve, and are not merging the results, since we need this to be a separate body.

   

10. Use Delete Face (Insert > Face > Delete) to patch the original face created by the Wrap feature to avoid issues with zero-thickness or edges that overlap one another repeatedly.

    

11. Select both Solid Bodies and use the Combine feature (Insert > Features > Combine) to subtract the swept body from the cylindrical body

    

At this point, you could fillet the straight face at the end to round it out, and it would be complete.

Now you have a CNC-happy swept cut on a cylinder. If we used the Wrap-Deboss method or used Cut-Extrudes, we would end up with a cut with incorrect inside faces, which would be inaccurate and not representative of what would happen if this were to be machined.

The attached 2015 & 2026 part files include all of the steps covered in this guide.

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.