How to Show Part Knurling in SOLIDWORKS – Part 1

Article by James Swackhammer updated May 10, 2021

Article

We all know what knurling is, right? The most common use for knurling is to add grip to an otherwise slippery part. Using this is done on a lathe, turned with special bits or tooling. Now, how do we get knurling on a SOLIDWORKS part?

Well, put on your swimming goggles because we are diving into the deep end with the hard method first.

Creating the physical cuts for knurling is a 4 step process:

Step 1: Helix/Spiral Path

  1. I have a handle of an eventual dumbbell. I want to add grip to the center. We need a Helix/Spiral for the knurling cuts to follow, this being the path. For a Helix/Spiral we need to have a sketch with a circle in it. The circular sketch can be as simple as grabbing the outer edge and doing a Convert Entities.
Add a reference plane for SOLIDWORKS Knurling sketch

I like starting where the knurling will begin, so I add a reference plane for my sketch.

 

  1. The Helix/Spiral is next and that is located in the Features tab under Curves. Activate the command and click on the circular sketch. Before putting in any dimensions I suggest choosing the correct direction, clockwise or counter clockwise.
I keep mine at a constant pitch and I have the pitch length lining up with the end of my knurling.

I keep mine at a constant pitch and I have the pitch length lining up with the end of my knurling.

Step 2: Create Profile for Cut

Create a profile to cut out. Similar to a loft or sweep we need a profile to cut. I have drawn a diamond shape using the 3 Point Center Rectangle command, making perpendicular lines equal and adding in one dimension.

 

Make sure to fully define the sketch with coincident relations to the handle profile.

Make sure to fully define the sketch with coincident relations to the handle profile.

Step 3: Sweep Cut

Come up for air the prep work is done, now we get to fun part. I advise saving your work here and almost every step after because the waves are rough with how taxing it is on the computer. Sweep Cut is located in the feature tab beside the Fillet command. Select your profile created in step 2 then select the path (Helix/Spiral) created in step 1.

Sweep Cut Profile

I have a few other options selected, like having the profile cut go Bidirectional, having the Profile Orientation set to Follow Path and Profile Twist set to Minimum.

Step 4: Pattern the Cut feature

  1. We can now we move onto the circular pattern. Nothing too special here other than selecting the Geometry pattern check box. This will improve the much needed performance for this part.
Save before you pattern

Before you pattern make sure you smash that Ctrl+S!

  1. To finish this off we need the cuts to cross each other, and for that we use a Mirror feature. Again, nothing too special here other than selecting the Geometry pattern and prepare for a slower part.
Pattern SOLIDWORKS Knurling Cut

This type of pattern can break computers if you are not running a decent or approved graphics card or enough ram.

SOLIDWORKS Knurling Completed

And there we have it, a part with physical cuts for knurling. The deep end wasn’t so bad, right? We didn’t drown, did we? Although, my computer felt like it took on water. Subscribe for the next article where I will show an easier faster way for knurling. Or attend a SOLIDWORKS Advanced Part Modeling online training course to learn more part techniques.

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James Swackhammer

James is a SOLIDWORKS Technical Support Application Expert based in the Javelin Oakville head office