How to model Bolt with terminating thread in SolidWorks?

Sudhir Gill

3 Mar, 2012 06:58 AM

Here is the tutorial.

1. Step 1:

   Top plane>>Sketch.
   

   

2. Step 2:

   Circle of 20mm dia.
   

   

3. Step 3:

   Extrude it by 100mm.
   

   

4. Step 4:

   Top face>>Sketch.
   

   

5. Step 5:

   Draw a polygon of 32.5mm circle.
   

   

6. Step 6:

   Extrude it by 10mm.
   

   

7. Step 7:

   Top face>>Sketch.
   

   

8. Step 8:

   Draw a circle of 32.5mm dia or tangent to the side of polygon.
   

   

9. Step 9:

   Extrude cut it by flip side to cut at 60º draft.
   

   

10. Step 10:

    Same cut with lower side of polygon.
    

    

11. Step 11:

    Chamfer the bottom edge by 2mm.
    

    

12. Step 12:

    Top plane>>Sketch.
    

    

13. Step 13:

    Select the outer edge and then convert entities.
    

    

14. Step 14:

    Make a helix defined by Height and Pitch with height=80mm, pitch=2mm Clockwise.
    

    

15. Step 15:

    Reference Geometry>>Plane.
    

    

16. Step 16:

    Offset the top plane by 80mm or by coincident to the helix end point.
    

    

17. Step 17:

    Plane1>>Sketch.
    

    

18. Step 18:

    Convert the sketch5 under previous helix.
    

    

19. Step 19:

    Create a helix with height=10mm, pitch=2mm clockwise at taper helix 30º outward.
    

    

20. Step 20:

    Right plane>>Sketch.
    

    

21. Step 21:

    Draw a triangle using polygon tool.
    

    

22. Step 22:

    Sweep cut the triangle about helix1.
    

    

23. Step 23:

    Select the end face of the sweep cut and then sketch.
    

    

24. Step 24:

    While selecting the face click convert entities.
    

    

25. Step 25:

    Sweep cut that sketch about helix2.
    

    

26. Step 26:

    And we have terminating threads.
    

    

27. Step 27:

    Rendered Image.