Tutorial - Creating knurl in SolidWorks?

Here is the tutorial.
Step 1:
Start SolidWorks in Part mode.
Step 2:
Top Plane>>Sketch.
Step 3:
Draw a circle of 70mm diameter.
Step 4:
Extrude it by 100mm.
Step 5:
Select chamfer tool.
Step 6:
Select both edge and chamfer it by 5mm at 45º.
Step 7:
Select the bottom face and then sketch.
Step 8:
Select the outer edge and then convert entity.
Step 9:
Select Helix and spiral under curves.
Step 10:
Change defined by to height and revolution. Enter 100mm height and 0.25 revolutions at 0º start angle. Click OK.
Step 11:
Top plane>>Sketch.
Step 12:
Select Polygon tool.
Step 13:
Enter number of sides 3 and draw it along piercing the helix. Exit the sketch.
Step 14:
Under features tab select swept cut.
Step 15:
Select the triangle as the profile and helix as the path.
Step 16:
Now reference geometry and then axis.
Step 17:
Select Top plane and origin as the references.
Step 18:
Now select circular pattern.
Step 19:
Select the axis as the parameter and the swept-cut as the feature to be patterned. Click OK.
Step 20:
Select mirror tool.
Step 21:
About Right plane or front plane mirror the circular pattern.
Step 22:
Click OK.
Step 23:
And we have the Knurl obtained.
Thank you!
Thanks for this !!
Well done, works like a charm!
worked great!
Don't know if I'll ever use it, but that was fun. Thanks.