Surfaces

This exercise is reproduced from Jan-Willem Zuyderduyn's "How to Model A Deodorant Roller in SolidWorks?" tutorial from LearnSolidWorks.com.


    Reference Images

  1. Make a Deodorant folder and download the files frontview_deoroller.jpg and sideview_deoroller.jpg to that folder.
  2. Start SolidWorks.
  3. Make a new part.
  4. Set the units to millimeters.
  5. Make a new sketch on the Right plane.
  6. Go to Tools > Sketch Tools > Sketch Picture and insert the sideview_deoroller.jpg image. Choose Low Resolution.
  7. Set the picture properties as follows:
  8. Close the sketch.

  9. Make new sketch on the Front plane.
  10. Go to Tools > Sketch Tools > Sketch Picture and insert the frontview_deoroller.jpg image. Choose Low Resolution.
  11. Set the picture properties as follows:
  12. Close the sketch.


    Cap

  13. Make a new sketch on the Right plane.
  14. Add two centerlines as shown.
  15. Add two line segments, and connect them with a spline without any midpoints.
  16. Add tangent relations between the spline and the line segments.
  17. Adjust the spline to match the reference image. You will only be able to change the lengths of the arrows, not the angles, due to the tangent relations.
  18. Close the sketch.
  19. Make sure the Surface tab is visible. If not, right click on any tab and select Surface.
  20. Create a Revolved Surface feature from the sketch.


    Body

  21. Create a new sketch on the Right plane.
  22. Draw the 53 mm line as shown. The bottom point should be horizontal to the origin.
  23. Close the sketch.
  24. Rename the sketch to GUIDELINE_FRONT.


  25. Create another sketch on the Right plane.
  26. Draw the 54 mm line as shown. The bottom point should be horizontal to the origin.
  27. Close the sketch.
  28. Rename the sketch to GUIDELINE_BACK.


  29. Create a new sketch on the Front plane.
  30. Draw a spline without midpoints as shown. The bottom point should be horizontal to the origin.
  31. Change the arrows to approximate the outline of the body.
  32. Close the sketch.
  33. Rename the sketch to GUIDELINE_SIDE.


  34. Create a new sketch on the Top plane.
  35. Draw a centerline connecting the front and back guidelines.
  36. Draw a closed oval spline with four points, three of which intersect the guidelines.
  37. Select the spline point not on a guideline, shift-click on the centerline, then shift-click on the opposite point (on the side guideline). Add a Symmetric relation.
  38. Close the sketch.
  39. Rename the sketch to PROFILE.


  40. Create a new sketch on the Right Plane.
  41. Draw a 58 mm line up from the origin.
  42. Close the sketch.
  43. Rename the sketch to PATH.


  44. Create a Swept Surface feature.
  45. Select the PROFILE sketch as the Sweep Profile.
  46. Select the PATH sketch as the Sweep Path.
  47. Select the three GUIDELINE sketches as the guidelines curves.
  48. Click OK.


    Trim the Top of the Body

  49. Create a new sketch on the Right plane.
  50. Draw the cut line as shown.
  51. Close the sketch.
  52. In the Surface tab, select Trim Surface.
  53. For the Trim Tool, select the sketch you just made.
  54. Choose Remove Selections.
  55. Set the Surface Split Options to Natural.
  56. Click on the part of the body above the trim line; it should turn orange.
  57. Click OK.


    Create the Neck

  58. Create a Lofted Surface feature.
  59. In the Profiles box, select the bottom edge of the cap and the top edge of the body.
  60. Make sure the green balls are aligned.
  61. Click on the Start/End Constraints box.
  62. Set both constraints to Curvature to Face.
  63. Change the length of the purple arrows to adjust the shape of the loft. Adjust it to match the profile in the image.
  64. Click OK.
  65. Turn off visibility of the sketches with the images.


    Fill the Bottom

  66. Create a Filled Surface feature.
  67. Click on the bottom edge of the body.
  68. Click OK.

    Knit the Surfaces and Create a Solid Body

  69. Create a Knit Surface feature.
  70. Select the cap, neck, body, and bottom surfaces.
  71. Turn on Create Solid.
  72. Turn on Merge Entities.
  73. Turn off Gap Control.
  74. Click OK.
  75. Fillet the bottom edge of the body with a radius of 2 mm.

    Cut the Cap Gap

  76. In the Features Tab, open Reference Geometry and create an Axis.
  77. Select the Cylindrical/Conical Face option.
  78. Click on the cylindrical (bottom) segment of the cap.
  79. Click OK.
  80. Create a new sketch on the Right plane.
  81. Draw the rectangular cutting profile as shown. Make sure the right edge extends past the end of the neck surface.
  82. Close the sketch.


  83. Insert a Revolved Cut feature using the sketch and the axis.


    Color and Save

  84. Color the cap turquise and the rest of the part white.
  85. Save the file as Deodorant.SLDPRT.
  86. Make a rendering of your part.