How to model Earphone in SolidWorks?

Sudhir Gill

16 Feb, 2012 05:10 PM

This tutorial illustrates how to model an earphone using surfacing methods. Since a lot of persons doesn't know about surfacing model therefore i tried to perform every function step by step. If you have any problem struggling with that even after my efforts, just let me know. I will help you as much as I can.

1. Step 1:

   Start Solidworks in Part mode. Select front plane and then sketch.
   

   

2. Step 2:

   Draw entity using splines like this one. For this sketch i have used two spline and a centre line along right plane. The two splines are having tangent relation.
   

   

3. Step 3:

   Now select revolve surface under surfaces tab. Revolve the profile along the centre line.
   

   

4. Step 4:

   Under surfaces tab select Reference geometry >> plane. Now select Right plane as the first reference and offset it by considerable distance.
   

   

5. Step 5:

   Now select plane1 and then sketch.
   

   

6. Step 6:

   Draw a circle like this one.
   

   

7. Step 7:

   Under sufaces tab click Extruded surface.
   

   

8. Step 8:

   Extrude it in both direction with a considerable distance.
   

   

9. Step 9:

   Now select front plane and then sketch.
   

   

10. Step 10:

    Draw two spline cutting the surfaces.
    

    

11. Step 11:

    Under surfaces tab select trim surfaces.
    

    

12. Step 12:

    Select the surfaces under the splines and remove them.
    

    

13. Step 13:

    Under surfaces tab select lofted surface.
    

    

14. Step 14:

    Select both edges.
    

    

15. Step 15:

    Under Start/End constraints change start and end constraint to tangency to face. Click OK.
    

    

16. Step 16:

    We have basic shape of the earphone. I have decreased the radius of the extruded surface Because it was a little larger.
    

    

17. Step 17:

    Select section view in standard views.
    

    

18. Step 18:

    Select front plane for section and click OK.
    

    

19. Step 19:

    Under surfaces tab select offset surface.
    

    

20. Step 20:

    Select the top face and change the distance to minimum i.e. about 1.5mm in my case.
    

    

21. Step 21:

    Now select Top plane and then sketch.
    

    

22. Step 22:

    Draw a circle.
    

    

23. Step 23:

    Under surfaces tab select trim surfaces.
    

    

24. Step 24:

    Trim the inner portion of the top-most face.
    

    

25. Step 25:

    Again top plane and then sketch.
    

    

26. Step 26:

    This time draw a circle considerably smaller than last one.
    

    

27. Step 27:

    Select trim surface under surfaces tab.
    

    

28. Step 28:

    Select the outer portion of the offsetted surface.
    

    

29. Step 29:

    Click OK and the area is trimmed.
    

    

30. Step 30:

    Under surfaces tab select boundary surface.
    

    

31. Step 31:

    Select both edges.
    

    

32. Step 32:

    Select tangency to face for both edges.
    

    

33. Step 33:

    Click OK.
    

    

34. Step 34:

    Now under surfaces or feature tab select reference geometry and then axis.
    

    

35. Step 35:

    Select top plane and origin. This will create an axis perpendicular to top plane and passing through origin.
    

    

36. Step 36:

    Now select top plane and then sketch.
    

    

37. Step 37:

    Make a circle for hole.
    

    

38. Step 38:

    Now click linear sketch pattern in sketch tab.
    

    

39. Step 39:

    Select the circle to entity to pattern.
    

    

40. Step 40:

    Adjust the distance and increase the number of instances.
    

    

41. Step 41:

    Now select circular sketch pattern.
    

    

42. Step 42:

    Now select the 2nd circle to pattern.
    

    

43. Step 43:

    Repeat the same step for other circles increasing the number of instances each time.
    

    

44. Step 44:

    Under surface tab select trim surface.
    

    

45. Step 45:

    Now select keep selection.
    

    

46. Step 46:

    Select the excluded surface of holes.
    

    

47. Step 47:

    Click OK and the surface is trimmed.
    

    

48. Step 48:

    Now select top plane and then sketch.
    

    

49. Step 49:

    Use slot tool to make 2 slots.
    

    

50. Step 50:

    Now select trim surface in surface tab and select remove selection. Select the surface bounded in slots and click OK.
    

    

51. Step 51:

    Now we have the space for the air.
    

    

52. Step 52:

    Select knit surface under surface tab.
    

    

53. Step 53:

    Select all surfaces one by one and then click OK.
    

    

54. Step 54:

    Under surface tab select thicken.
    

    

55. Step 55:

    Select the surface. It will select Knit surface feature. Change the thicken distance to 1mm and outside direction. Click OK.
    

    

56. Step 56:

    Now we have solid body of the earphone. We will now seperate the bodies.
    

    

57. Step 57:

    Select top plane and then sketch.
    

    

58. Step 58:

    Change view to hidden with shaded line.
    

    

59. Step 59:

    Offset the edge by 0.50mm and then draw two straight line horizontally. Trim other entities.
    

    

60. Step 60:

    Select revolved surface in surface tab.
    

    

61. Step 61:

    Select axis1 and click OK.
    

    

62. Step 62:

    Go to insert menu then feautres >> split.
    

    

63. Step 63:

    Select the revolved surface as the trim tool and click cut part.
    

    

64. Step 64:

    Now check both the bodies and click OK. This feature will generate two split bodies by the revolved surface.
    

    

65. Step 65:

    Now hide the revolved surface.
    

    

66. Step 66:

    Again select section view about front plane in standard view toolbar.
    

    

67. Step 67:

    Select reference geometry and then plane under surface or features tab.
    

    

68. Step 68:

    Select top plane and then offset it by a distance so that it will lie in the upper body.
    

    

69. Step 69:

    Select the plane2 and then sketch.
    

    

70. Step 70:

    Draw a circle larger than the region bounded by the holes.
    

    

71. Step 71:

    Under features tab click extruded boss/base feature.
    

    

72. Step 72:

    Under direction1 select up to body.
    

    

73. Step 73:

    Select the upper body and enable thin feature by a distance of 0.50mm. Click OK.
    

    

74. Step 74:

    Now we have the body for the speaker of ear phone.
    

    

75. Step 75:

    Now click file save.
    

    

76. Step 76:

    Enter any file name for the part document. I entered earphone for myself.
    

    

77. Step 77:

    After saving part click insert>>feature and then split.
    

    

78. Step 78:

    Again select revolved surface2 from the surface bodies under tree view and click cut part.
    

    

79. Step 79:

    Double click the cut body1 and save it.
    

    

80. Step 80:

    Repeat the same step for the other body and click OK.
    

    

81. Step 81:

    Now right click the split2 feature and then select create assembly.
    

    

82. Step 82:

    Click browse.
    

    

83. Step 83:

    Now save the assembly file for the splitted part document.
    

    

84. Step 84:

    Now the assembly file will open.
    

    

85. Step 85:

    Right click the upper body and select float.
    

    

86. Step 86:

    Move it and then rotate it to have a better view.
    

    

87. Step 87:

    Here is the rendered image of the earphone. This one is not much better than the last one but you can make one better if done with care.