Knurling in SOLIDWORKS

Knurling in SOLIDWORKS
Posted in: Mechanical Design
March 15, 2017

Knurling is a type of surface finish commonly desired on precision tools and other instances where additional hand grip is required on a machined part. In practice, knurling is achieved by pressing a dedicated knurling tool into the rotating workpiece. For this reason, it may not be necessary for manufacturing purposes to model the knurling explicitly in CAD- many times a simple callout on a drawing for a knurled surface may suffice.

If it’s desired to have an accurate representation of the product in CAD for purposes such as photorealistic rendering, however, then it may be necessary to model the actual knurled geometry. This article and companion video will focus on a technique to achieve this, and some performance considerations.


The first step to creating the knurled surface finish is to create a sketch to represent the knurl tool profile. In this example, I used a diamond shape placed with its center coincident to the outer diameter of the cap, and the width controlled by an angle dimension of 5 degrees. Compare against your particular knurl tool for specifics.

The second ingredient required is a helical path, which the profile will eventually be swept along for a cut. To create the helical path, first create a sketch on the same plane used to create the profile, and Convert Entities of the outside edge of the cylinder. It is important that this sketch only contains a single circle.

Creating a Helical Path

Then, use the Helix/Spiral feature under Features -> Curves -> Helix/Spiral and select the sketch containing the circle. Use the Helix option and adjust the start angle and pitch values to align the Helix with the profile. In this example, the profile was aligned vertically with the origin, which aligned with a start angle of 180 degrees. The profile could alternatively be sketched after generating the Helix to ensure they line up.

Once the profile and path are created, create a Swept Cut feature using these selections and the “Minimum Twist” option.

All that is left then is to Mirror and Circular Pattern the resulting Swept Cut to produce a representation of the desired surface finish.

Adding Finish

Generating textured surfaces by cutting away at the CAD geometry is a computationally intensive process. To help minimize rebuild times there are two key settings to pay attention to. The first is in the Circular Pattern options. Use the option for Geometry pattern which can reduce rebuild times significantly for repetitive geometry.

The second option is a System Option accessible under the Performance tab called Verification on rebuild.  Verification on rebuild can drastically increase rebuild times on geometry such as this as it performs more advanced geometry checks between each set of faces. It is recommended to disable it on these types of parts or you may experience excessive rebuild times.

Geometry Pattern and Verification

Also consider grouping these detail features together so they can easily be suppressed. Whenever adding cosmetic detail like this, it is desirable to also create a “simplified” configuration in case performance ever becomes an issue- for instance, if dozens of these knurled pieces were necessary for a large assembly.

There may also be alternative “lightweight” ways to represent the textured surface, such as using a custom appearance with a Displacement Map. However, this effect would only be visible in a photorealistic rendering – not within SOLIDWORKS CAD.

For additional details on how this process can be performed, please check out this YouTube video or see what else we have on our channel, check out our SOLIDWORKS page or Get a Quote for SOLIDWORKS 3D CAD. Don't hesitate to contact us at Hawk Ridge Systems today!

March 15, 2017
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Kristo Philpott
March 22, 2017
Excellent post. I certainly appreciate this website. Keep it up!

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