Saturday, January 13, 2018

Autodesk Inventor 2018 Tutorial || Spring|| Along with captions and audio narration

Spring

In this tutorial we will learn to create a model of a ‘Spring’ using Autodesk Inventor software. To create this model we will utilize various part modelling features like 2D and 3D sketching, Coil, Sweep, Circular Pattern etc.

 

Video Transcription

  1. Start a new part file using the metric template.
  2. Create a sketch on the XY plane along with dimensions and proper constraints in the following way.
  3. The sketch is complete and it is a fully constrained sketch so exit from the sketching mode.
  4. Activate Coil Tool.
  5. The profile for the coil is automatically selected.
  6. Define centreline of the sketch as Axis.
  7. Switch to Coil Size tab and select Pitch and Height as the type of coil.
  8. Fill 50 mm as pitch and Height will be equal to the length of centreline.
  9. Flip the direction of the coil and execute the command.
  10. Turn off the model shadow and change the colour of the model as per your wish.
  11. Make some changes in the lighting settings to see the model clearly.
  12. After all these settings set the current view as home view using the View Cube.
  13. Save the file with the name Spring.
  14. The spring created so far can also be created using the helical curve and sweep tool. Let us see how to do so.
  15. Select sketch 1 from the browser bar and activate share sketch option from the right-click menu.
  16. Drag the end of the part above the coil feature to suppress it.
  17. Create a new 3D sketch.
  18. Activate Helical Curve Tool.
  19. Select Pitch and Height as the type of Helical Curve.
  20. Fill 50 mm as pitch value.
  21. Next, define start point of helix axis and then end point of the helix.
  22. Click the centre point of the circle to define start point of the helix.
  23. Activate rotation as clockwise and execute the command.
  24. Exit from the 3D sketching environment.
  25. Activate Sweep tool.
  26. The profile for the Sweep is automatically selected.
  27. Select Helical Curve as a path for the sweep and execute the command.
  28. Turn off the visibility of sketch 1.
  29. Switch to left view using view cube and create a new sketch on YZ plane.
  30. Activate isometric view and take the project of the following face of the model.
  31. Convert the project line into construction geometry and switch back to the left view.
  32. Draw a centre point arc in the following way.
  33. Align ends of the arc with the centre of arc using horizontal and vertical constraints.
  34. Apply a dimension of 75 mm over the arc and exit from the sketching mode.
  35. Switch to the front view and create a sketch over XY plane.
  36. Take the project of the following edge of spring and the arc drawn in the previous sketch.
  37. Convert the projected sketch into construction geometry.
  38. Keep changing the views of the model as shown here to draw an accurate sketch.
  39. Turn off the visibility of Sketch 2.
  40. Daw an arc using 3 point arc tool connecting these two points and apply tangent mate over the arc as shown.
  41. The sketch is complete so exit from the sketching mode.
  42. Activate Extrude Tool.
  43. Select Surface as the Output type.
  44. In the extents field select distance and symmetric option.
  45. Select the profile and drag the surface as shown.
  46. Click Ok to execute the command.
  47. Turn on the visibility of Sketch 2.
  48. Start 3D sketch Command.
  49. Here activate Project to surface tool.
  50. First, select the surface and then the curve which we want to project.
  51. Click Ok to execute the command.
  52. Here is our projected curve.
  53. Turn off the visibility of Sketch 2 and surface extrude 1.
  54. Create a new sketch over the following face of the mode as displayed.
  55. Activate Sweep Tool.
  56. The profile is automatically selected so define the path and execute the command.
  57. Set the view of the model as displayed here.
  58. Activate Circular Pattern Tool.
  59. First, select sweep feature then define X axis as rotational axis.
  60. Fill value 2 in Occurrence Count and 360° in Occurrence Angle.
  61. Click ok to execute the command.
  62. Our model is complete hence save the file.

download-Link

 

Visit the following link to get the model file…
http://autode.sk/2CWtjfe

 

 

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Visit the following link to watch basic tutorial on Autodesk Inventor by us

https://www.youtube.com/playlist?list=PLb-IhKRMYSERYpB48aY-sZ10fN6CfXIL4

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To watch detailed tutorials on the same software visit the following link

https://www.youtube.com/playlist?list=PL74BDF7431ED13443

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