Tutorial - Making a bolt in Solidworks?

Sudhir Gill

3 Feb, 2012 03:29 AM

Here is the Tutorial. The attached file is the final output.

1. Step 1:

   Start Solidworks.
   

   

2. Step 2:

   Right Plane>>Sketch.
   

   

3. Step 3:

   Make a polygon circumscribed with circle dia 18mm.
   

   

4. Step 4:

   Extrude it by 7mm.
   

   

5. Step 5:

   We have the extruded polygon.
   

   

6. Step 6:

   On the right plane of the polygon start a sketch. Normal View to sketch.
   

   

7. Step 7:

   Make a circle tangent to the sides of polygon.
   

   

8. Step 8:

   Under features tab select Extruded Cut.
   

   

9. Step 9:

   Change extrude depth to 7mm. The draft angle to 60degree and check the flip side to cut. Click OK.
   

   

10. Step 10:

    Now you can see the polgon has rounded edges.
    

    

11. Step 11:

    Repeat the same steps for the other face also.
    

    

12. Step 12:

    Click on the right side circular face of the polygon and select sketch.
    

    

13. Step 13:

    Make a concentric circle of dia 16.6mm.
    

    

14. Step 14:

    Extrude it by 0.60mm.
    

    

15. Step 15:

    Select the circular face of the extruded body in previous step and select sketch.
    

    

16. Step 16:

    Make a circle of 12mm dia concentric to previous one.
    

    

17. Step 17:

    Extrude it by 50mm.
    

    

18. Step 18:

    Now we have the basic body of the bolt.
    

    

19. Step 19:

    Under features>>fillet arrow>>Chamfer.
    

    

20. Step 20:

    Select the circular edge of the bolt.
    

    

21. Step 21:

    Change chamfer settings to 1mm distance and 45degree.
    

    

22. Step 22:

    Now we have the chamfered body.
    

    

23. Step 23:

    Select this face and sketch.
    

    

24. Step 24:

    Under Sketch Tab choose convert entities.
    

    

25. Step 25:

    Select this edge and then click OK.
    

    

26. Step 26:

    Again click OK to exit convert entities.
    

    

27. Step 27:

    Under Features tab>>Curves>>Helix and Spiral.
    

    

28. Step 28:

    Choose Defined by Height and Pitch. Change the Height Value to 46mm and pitch value to 1.75mm keep other settings default.
    

    

29. Step 29:

    Click OK and we can see that helix has been creted.
    

    

30. Step 30:

    Top Plane>>Sketch.
    

    

31. Step 31:

    Make a equilateral triangle of side 1.7mm with one point coincident to the edge of the bolt.
    

    

32. Step 32:

    Under Features tab choose Swept cut.
    

    

33. Step 33:

    Choose the triangle sketch as profile.
    

    

34. Step 34:

    Choose helix as the path of the swept cut. Click OK.
    

    

35. Step 35:

    Now we are done, we have the bolt created.