In this tutorial, you will find a step by step guide on how to create a bevel gear in SolidWorks by using 3D features. I recommend that you play around and try to create different cogs and gears. Since almost all mechanical designs use gears and cogs they are very useful to know. A bevel gear might not be the most normal cog but it’s still a very important part.


Time required: 60 minutes
Difficulty: Beginner
Software: SolidWorks

There’s no specific exercise for this tutorial, the tutorial is an exercise in itself.

Looking for more exercises? Click here!

1. Open SolidWorks.

2. Open new part file.

  • Click new  Create a new document
  • Double click part  Creating a new partin the new tab to create a new part document.

3. Select right plane, and click sketch  Create a new sketch

  • To have a normal view on the selected plane, choose normal to  Normal to selected planefrom the click options.
  • You can also press space on your keyboard, to see the orientation panel. Then choose normal to.

4. On the sketch tab, click on line tool.
5. Using the line tool, click on the origin  Originand draw the following geometry lines by using the SolidWorks horizontal, vertical, parallel and normal guidelines.



6. Click smart dimensions  Smart dimensions in solidworks

7. Dimension the geometry according to the example. Make sure it is fully defined.


8. Save and exit the sketch mode.

9. Select features toolbar.

10. Select sketch1  sketch-1from the part tree.

11. Click revolved boss/base  Revolved Boss - Revolved BaseThe revolve window will appear.


12. Click on the axis of revolution tab, then select L1 as the rotation axis.



13. Make sure that your angle is set to 360 degrees, and click ok.


14. Select front plane and click sketch.

15. On the sketch tab, click on the line tool.

16. Choose the centerline option.


17. Using the centerline tool, draw a line which passes through origin.


18. Draw another line according to the example.


19. Select L2 line and the E1 by holding the ctrl key at the time. The property manager window will now appear.

  • The property manager window enables you to set different constraints and relation between entities.


20. In the properties window, select the collinear  center-line-solidworksas a relation between these.


21. Press ok.


22. Save and exit the Sketch mode.

23. Click insert  inserton main toolbar

24. Go through insert -> reference geometry and select plane  reference-geometry-2


25. In the property manager, click first reference then select face1 as a tangent face from the screen.



26. In the property manager, click second reference  second-referenceand select L2 as a perpendicular line from the screen.

27. Select plane1 (the plane was created in the previous steps), and click sketch.


28. Press ok to insert the geometry plane.

29. On the sketch tab, click on line tool. Choose centerline  Center Line Iconoption.

30. Using the centerline tool, draw a line which almost overlay the previous centerline.


31. On the sketch tab, click on line tool.

32. Using the line tool, draw the following geometry.


  • The line tool can be used to draw different curves. For this purpose click on the screen for the starting point and then move back to the starting point and start to draw a curve.


33. Click smart dimensions.

34. Dimension the geometry according to the example.


35. Click on mirror entities  mirror-entities

  • Mirror entities mirrors pre-existing 2D sketch entities on a plane around the selected line/centerline entity.

36. In the property manager, select the centerline as the mirror about. Select the drawn lines and curves as the entities to mirror.



37. Press enter to place the mirror shape.


38. Save and exit sketch mode.

39. Select the features toolbar.

40. Click extruded-cut  extruded-cutThe extrude-cut window will now appear.

  • Extruded-Cut is a 3D feature which helps you to remove materials from the 3D model. You can cut in both directions and you are able to cut in angled extrusion by checking the draft option

41. Use the previous sketch as selected contours selected-contours

42. Select up to next as the depth of cut 71_5


43. Check the draft  draft-featurefeature, and set the angle to 4 degrees.


44. Press enter.


45. On the features tab, click on the linear pattern toolbar listlinear-patternand select circular pattern circular-pattern


  • 3D pattern is a SolidWorks feature which helps you to remake features on a predefined pattern, such as lines, circles, curves, etc.
  • 3D circular pattern is a 3D pattern feature which enables you to create the circular pattern using the feature you select as the seed feature.

46. In the property manager, select your extrude-cut as a features to pattern.


47. Set the angle parameter to 360 degrees.


48. Set the number of patterns to 25.


49. Check the equal spacing box.



50. Press enter.


51. Click on the upper surface of the disk, and select sketch.


52. Using the circle tool, draw a circle centered at origin.


53. Dimension the circle by using the smart dimension, accordingly.


54. Save and exit sketch mode.

55. Click cut-extrude. The extrude-cut window will now appear.

56. Select the previous sketch as selected contours.

57. Select up to next as the depth of cut  71_5


58. Press enter, you should now see a complete bevel gear in 3D!


59. Click file.

60. Click save.

Exercise 5 – Creating a bevel gear



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