# Modeling a Helical Cut on a Cylinder in SOLIDWORKS

One of the frequent questions we get in support is modeling accurate swept cuts on a cylinder. Use the following technique for accurate tool-body cuts.

Like all sweeps, the important elements are the path, profile, guide curves, and controlling options.

Let's start with the path. We'll begin with a simple 2D sketch that gets wrapped around the cylindrical face.

Next is wrapping it using the scribe option, creating 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.

Now that we have the foundational geometry developed, the next steps require some surfacing techniques. Don't be afraid of surfacing! If there were an easier way, then we would use it. So now that we have the outline of the cut on our cylinder, we need to obtain a centerline of that outline to use as our path.

Use a Ruled Surface along one side of the outline using the Normal to Surface option.

Next we need to extend the bottom edge of that surface slightly (by .01” here) so that it intersects the cylindrical body. Being tangent is not enough for the next step.

Now we just need to offset this surface .2" since the overall width of the slot is .4".

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 and select the surface body and the face and use Intersection Curve.

With that last step completed, we have successfully created the path of our sweep. The next step, creating the profile, is simple. Draw a rectangular profile normal to the end of the path.

Now you have the required selections for your sweep: the profile, the path, and the guide curves. The guide curves are going to be 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 quite 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.

With the Swept-Boss completed, there are only two features left to complete the design. We first need to Delete and Patch the original face created by the Wrap feature, to avoid issues with zero-thickness or edges that overlap one another repeatedly.

With the face deleted and patched (now it is a smooth cylindrical face) we can use the Combine feature and 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 part file includes all of the steps covered in this guide.