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Tutorial - Creating knurl in SolidWorks?

By Sudhir Gill on 20 Feb 15:49 2 answers 7096 views 6 comments

Tutorial on creating knurl in SolidWorks.

2 answers

  • Sudhir Gill
    Sudhir Gill over 2 years ago

    Here is the tutorial.

    1. Step 1

      Start SolidWorks in Part mode.

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    2. Step 2

      Top Plane>>Sketch.

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    3. Step 3

      Draw a circle of 70mm diameter.

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    4. Step 4

      Extrude it by 100mm.

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    5. Step 5

      Select chamfer tool.

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    6. Step 6

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

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    7. Step 7

      Select the bottom face and then sketch.

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    8. Step 8

      Select the outer edge and then convert entity.

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    9. Step 9

      Select Helix and spiral under curves.

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    10. Step 10

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

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    11. Step 11

      Top plane>>Sketch.

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    12. Step 12

      Select Polygon tool.

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    13. Step 13

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

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    14. Step 14

      Under features tab select swept cut.

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    15. Step 15

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

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    16. Step 16

      Now reference geometry and then axis.

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    17. Step 17

      Select Top plane and origin as the references.

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    18. Step 18

      Now select circular pattern.

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    19. Step 19

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

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    20. Step 20

      Select mirror tool.

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    21. Step 21

      About Right plane or front plane mirror the circular pattern.

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    22. Step 22

      Click OK.

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    23. Step 23

      And we have the Knurl obtained.

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  • jairo luis
    jairo luis over 2 years ago

    muy bien ese moletado amigo

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