Monday, December 9, 2013

Autodesk Inventor Modelling and Animation Tutorial--‘Hinge’ (with caption and audio narration)



Serial No. 49

Autodesk Inventor Modelling and Animation Tutorial--‘Hinge’ (with caption and audio narration)


Click the following link to get the model file: -


Transcription of Video

Hinge Modelling and apply motion in it through Drive-Constraint.

  1. Create a New ‘Standard (in).ipt’ Part file.
  2. Sketch1 is active by default.
  3. Draw a Rectangle 1.25 in. x 0.0625 in., coincident with Auto project part origin.
  4. Draw a Circle of 0.375 in. diameter.
  5. Apply a Tangent Constraint between circle and base line of the rectangle.
  6. Apply a Vertical Constraint between centre point of Circle and Auto project part origin.
  7. Draw another Circle of 0.25 in. diameter, Concentric with the previous one.
  8. Finish the Sketch.
  9. Start the Extrude command, select rectangle and the profile formed between the two circles.
  10. Enter the distance value 5 in. and select Symmetric option in the direction field.
  11. Click OK.
  12. Change the existing colour of the part into Popcorn.
  13. Save the file with the name Part 1.
  14. Create a new work plane 1 in. away from the front face of part.
  15. Start a new sketch on this Work Plane.
  16. Take the project of this edge of the part with Project Geometry Tool.
  17. Right click in the design window and select Slice Graphic from the context menu.
  18. By doing so hidden sketches behind the part will be seen clearly.
  19. Draw two lines to close the profile.
  20. Finish the Sketch.
  21. Start the Extrude command. It will automatic select the last drawn sketch profile, choose Cut option to remove the material from the part.
  22. Enter the distance value 1 in.
  23. Click ok.
  24. Start the Rectangular Pattern tool.
  25. Select Extrusion2 in the design window as feature.
  26. Click the ‘Direction 1’ button, and then select the outer edge of the Part1.
  27. Enter the value 2 in the column count input box.
  28. Enter the value 2 in. in the column spacing input box.
  29. Click OK.
  30. Take the project of edges of the model.
  31. Draw a rectangle coincident with the end point of the projected lines.
  32. Start the Offset tool, select the rectangle and drag the profile inside.
  33. A new Rectangle will be created.
  34. Place the dimension .25 in. as offset distance between the two rectangles.
  35. Start the Rectangular Pattern tool.
  36. Select bottom line of the rectangle.
  37. Click the ‘Direction 1’ button, and then select the vertical line of the rectangle. Click Flip button to change the direction of pattern.
  38. Enter the value 4 in the column count input box.
  39. Click the arrow button to expand the input choices in the column spacing input box.
  40. Choose ‘Measure’ option then select the vertical line of rectangle.
  41. Click more button to expand the dialogue box.
  42. Select ‘Fitted’ option and click OK.
  43. Convert all sketches into construction geometry.
  44. Hold the Ctrl Key and select the end points of these lines and convert them to centre point.
  45. Start the Hole Tool. The Points which we converted into centre point will be automatically selected.
  46. Set the diameter of the hole to 0.125 in.
  47. In the termination drop down menu select Through All option and Click OK.
  48. Start the Chamfer Tool.
  49. Select the top edges of all the holes.
  50. Enter the value 1/32 in. in the Distance field.
  51. Click OK.
  52. Save the file.
  53. Save As the same file with the name Part 2 also.
  54. This file will be used later in creation of Hinge Assembly.
  55. Close the file.
  56. Create a New Standard (in).iam Assembly file.
  57. Place the ‘Part 1’ file in the Assembly with aid of Place Component Tool.
  58. Save the Assembly with name ‘Hinge’.
  59. Place the ‘Part 2’ in the Assembly.
  60. Align ‘Part 2’ in correct position by using Rotate Component Tool.
  61. Some modifications are needed here in ‘Part 2’, so as to match it with Part 1.
  62. Select the Part 2 and double click it, to edit in the part modelling environment.
  63. Edit the Extrusion2 feature in the Browser Bar by double clicking it.
  64. In the Extrude2 dialogue box, change the direction of extrusion.
  65. In the same way, edit the Rectangular Pattern1.
  66. In the Column count input box, enter the value 3 and click OK.
  67. Click the Return icon, to return back in the Assembly modelling environment.
  68. Apply a mate constraint between the Axis of Part 1 and Part 2.
  69. Apply a Flush mate between the Front face of Part 1 and Part2.
  70. Right Click in the design window and select Create Component Tool from the marking menu.
  71. Give name of the part as ‘Centre Pin’.
  72. Click Ok.
  73. Select XY plane of Assembly, as a base plane for the new component.
  74. At present sketch1 is active of newly created Centre Pin.
  75. Take the project of edge of the hole.
  76. Finish the sketch.
  77. Start Extrude command. The sketch profile is automatically selected.
  78. In the extents drop down menu, select Between option.
  79. Select front face of part and then rear face of the part.
  80. Click ok.
  81. Change the model colour to Popcorn to distinguish it more clearly.
  82. Create a new sketch on the YZ plane of the Centre Pin.
  83. Take the project of front edge of the Centre Pin.
  84. Activate Slice Graphic Command from the Right click context menu.
  85. Draw a Three Point Rectangle, coincident with the midpoint and end point of the projected line.
  86. Apply a horizontal dimension of 0.03125 in. on the rectangle.
  87. Draw a Thee Point Arc inside the rectangle.
  88. Finish the sketch.
  89. Start Revolve command, first select the sketch profile and later the axis.
  90. Click OK.
  91. Start the Mirror Command from the Pattern Panel of the Model Tab.
  92. Select Revolve1 feature in the browser bar.
  93. Select Mirror Plane button in the Mirror dialogue box, then select XY plane of Centre Pin.
  94. Click Ok and return back to the assembly.
  95. Change the view of Assembly by using View Cube.
  96. Apply an Angle Constraint between Part1 and Part2, to show the motion in the Assembly of ‘Hinge’.
  97. Activate an Angle Constraint, first select the top face of Par1, then top face Part2, at last select the front face Part2.
  98. Click OK.
  99. Set the browser Assembly View to Modelling View using the toggle at the top of the Browser Bar.
  100. Select the Angle:1 constraint under Constraints folder in the Browser Bar and change its name as ‘Drive’ by clicking twice slowly.
  101. Right click the ‘Drive’ Constraint and select Drive Constraint from the context menu.
  102. In the Drive Constraint dialogue box, set End value to 191.42 deg.
  103. Click more button to expand the dialogue box and set the value for Increment 0.25 deg.
  104. In the Repetitions field select Start/End/Start and enter value 2.
  105. Clear the screen by activating the Clean Screen command, Click the Forward Button to display the motion in the ‘Hinge’ Assembly.