Tutorial - Creating knurl in SolidWorks?

Sudhir Gill

20 Feb, 2012 04:01 PM

Here is the tutorial.

1. Step 1:

   Start SolidWorks in Part mode.
   

   

2. Step 2:

   Top Plane>>Sketch.
   

   

3. Step 3:

   Draw a circle of 70mm diameter.
   

   

4. Step 4:

   Extrude it by 100mm.
   

   

5. Step 5:

   Select chamfer tool.
   

   

6. Step 6:

   Select both edge and chamfer it by 5mm at 45º.
   

   

7. Step 7:

   Select the bottom face and then sketch.
   

   

8. Step 8:

   Select the outer edge and then convert entity.
   

   

9. Step 9:

   Select Helix and spiral under curves.
   

   

10. Step 10:

    Change defined by to height and revolution. Enter 100mm height and 0.25 revolutions at 0º start angle. Click OK.
    

    

11. Step 11:

    Top plane>>Sketch.
    

    

12. Step 12:

    Select Polygon tool.
    

    

13. Step 13:

    Enter number of sides 3 and draw it along piercing the helix. Exit the sketch.
    

    

14. Step 14:

    Under features tab select swept cut.
    

    

15. Step 15:

    Select the triangle as the profile and helix as the path.
    

    

16. Step 16:

    Now reference geometry and then axis.
    

    

17. Step 17:

    Select Top plane and origin as the references.
    

    

18. Step 18:

    Now select circular pattern.
    

    

19. Step 19:

    Select the axis as the parameter and the swept-cut as the feature to be patterned. Click OK.
    

    

20. Step 20:

    Select mirror tool.
    

    

21. Step 21:

    About Right plane or front plane mirror the circular pattern.
    

    

22. Step 22:

    Click OK.
    

    

23. Step 23:

    And we have the Knurl obtained.