In most situations, creating cuts as solid features, a Boolean function, is the most efficient method when working with solid bodies. This efficiency applies both in creating the actual feature, and the regeneration / rebuild time. However, there are some modeling situations in 3-D CAD where a solid cut does not work, but substituting a surface cut is a viable solution.

Diamond Knurl with flats (Pro-E)

One specific case is when attempting to create an intersecting solid cut through a helical / spiral sweep cut.  One of the two cuts will fail depending on the order of the features, and re-ordering the features will only change which cut will fail, and which one will succeed. I have noticed the problem in both SolidWorks and Pro/Engineer even though each uses a different geometric modeling kernel (SolidWorks –> Parasolid, Pro-E –> Granite).

For example, modeling a diamond knurl feature in Pro-E creates a very “heavy” part file, and is probably unnecessary in most cases. A better approach would be to add a knurl texture (JPEG image) to the part file and attach a note calling out the diamond knurl.  However, for demonstration purposes, a diamond knurl is modeled in this Pro/Engineer part file. After the diamond knurl feature, a flat needed to be created on the end of the part, which is done by removing an area of the diamond knurl (patterned helical sweep cuts). To accomplish this, a surface cut was used in-place of a solid cut.

Cut-with-Surface (SolidWorks)

When working with surfaces, be sure to extend the surface beyond the boundaries of the solid body. This mix of solids and surfaces is typically referred to as hybrid modeling (both solids & surfaces).  In Pro-E, I created an external sketch (before the spiral cut) of the excess material to be cut-away, and then created an extruded surface after the spiral / helical cut. To cut-away the excess material, select the cutting surface and “Solidify” (Edit –> Solidify). Be sure to select the remove material option and direction in the solidify feature.

In SolidWorks, it is basically the same produce except that you use “Cut with Surface” in-place of “Solidify” (Pro-E). Repeating what was previously mentioned, when working with surfaces, it is very important to let the surface extend beyond the edge of the solid part in-order to successfully cut-away the excess material. The attached images should be sufficient to guide you through the process.

In summary, the only reliable technique I have found when creating helical sweep cuts with intersecting cuts is to use a surface cut in-place of a solid cut for the intersecting cut. I hope you have found this information to be helpful.

Spring plunger with flats (SolidWorks)