Tutorial on creating knurl in SolidWorks.
Here is the tutorial.
Start SolidWorks in Part mode.
Draw a circle of 70mm diameter.
Extrude it by 100mm.
Select chamfer tool.
Select both edge and chamfer it by 5mm at 45º.
Select the bottom face and then sketch.
Select the outer edge and then convert entity.
Select Helix and spiral under curves.
Change defined by to height and revolution. Enter 100mm height and 0.25 revolutions at 0º start angle. Click OK.
Select Polygon tool.
Enter number of sides 3 and draw it along piercing the helix. Exit the sketch.
Under features tab select swept cut.
Select the triangle as the profile and helix as the path.
Now reference geometry and then axis.
Select Top plane and origin as the references.
Now select circular pattern.
Select the axis as the parameter and the swept-cut as the feature to be patterned. Click OK.
Select mirror tool.
About Right plane or front plane mirror the circular pattern.
And we have the Knurl obtained.
I've tried this long back when i started to learn SW , n i must say after doin this software got veerrrry slow :)
Just used it on a test gage and it worked great.
You can use a picture as a texture. I will let you know it when i'm done.
muy bien ese moletado amigo