Wednesday, November 27, 2013

Chain-Inventor Studio (Autodesk Inventor 2012)

Chain-Inventor Studio

Serial N0. 17

Chain-Inventor Studio (Autodesk Inventor 2012)
Video Tutorial with Caption and Audio Narration
This video displays a setting up of 61 chain links and 2 sprockets along a defined paths in Autodesk Inventor’s Assembly modelling environment.  First of all some base sketching afterward some advance pattern, adaptive features and assembly mates are to be applied to set up an animation matching the real world scenario… Later the whole mechanism consisting of required mates are driven by using Inventor Studio functionality of the software……
 


download-Link 

Click the following link to get the model file: - http://a360.co/115hj6r

 

 

 

 

Transcription of Video

Display of motion in Chain along with Sprocket through Inventor Studio
In this exercise here three pre-constructed Parts are selected for use, one is ‘Chain-Link’ and the other two Parts are Sprocket-Large and Sprocket-Small.
  1. Create a New ‘Standard (mm) .ipt’ Part file.
  2. At present Sketch 1 is active by default.
  3. Use the Finish Sketch command to exit from sketching mode.
  4. Open the visibility of YZ Work Plane under the origin folder in the Browser Bar.
  5. Click the Home icon on the View Cube to see the Design Window in Isometric View.
  6. Create a new Work Plane Parallel to YZ Plane at an offset distance of 320 mm.
  7. Create a new Sketch on XY Plane.
  8. Draw a Circle of 100 mm diameter, coincident with the auto projected part origin.
  9. Create another Circle of 75 mm diameter. The distance between these two circles will be 320 mm.
  10. Take the project of X Axis and convert it to construction geometry.
  11. The centre of small circle will be 12.5 mm below the projected X Axis line.
  12. Draw a line connecting top of two circles as displayed.
  13. Draw another line between two circles.
  14. Apply a Horizontal Constraint on it.
  15. Erase the unwanted sketches by using the Trim tool.
  16. Apply dimensions as displayed to fully constraint the sketch.
  17. Take the project of YZ Plane and Work Plane1 from the browser bar, with use of Project Geometry tool.
  18. Convert these projected lines into construction geometry.
  19. Apply a dimension between them. This dimension will be driven dimension.
  20. Now the sketch is complete, exit the sketch environment.
  21. Create a Work Point at the intersection of YZ Plane and bottom line of the sketch.
  22. Activate the Parameters tool from the Parameters Panel of the Manage tab.
  23. Create a User defined Parameter named ‘start’ by clicking ‘Add Numeric’ button in the Parameters dialog box.
  24. Click the ‘Equation’ column and then select the driven dimension in the design window.
  25. Click Done.
  26. Save the Part file with the name ‘Master’.
  27. Start the Rectangular Pattern Tool and select Work Point1 in the Browser Bar.
  28. Click the ‘Direction 1’ button and select the sketch in the design window.
  29. In the Column spacing input box, click arrow button to expand choices.
  30. Select List Parameters then select the ‘start’.
  31. Click the more button to expand the dialogue box.
  32. Select Adjust in the ‘Compute’ option.
  33. Click the Start button in the ‘Direction 1’ field and select the Work Point1 in the Browser Bar.
  34. Click OK.
  35. Open the visibility of Sketch2 from the Browser Bar.
  36. Select Work Plane1 in the Browser Bar and make it ‘Adaptive’ from the context menu.
  37. Activate Rectangular Pattern Tool once again.
  38. Select Work Point2 in the Browser Bar.
  39. Click the ‘Direction 1’ button and select the sketch in the design window.
  40. In the Column Count input box, enter the value 61.
  41. Click this drop down to specify pattern length.
  42. Select ‘Curve Length’ option.
  43. Click the more button to expand the dialogue box.
  44. Select Adjust in the ‘Compute’ option.
  45. Click the Start button in the ‘Direction 1’ field and select the Work Point2.
  46. Select Direction1 in the ‘Orientation’ option.
  47. Click OK.
  48. Save the file and close it.
  49. Create a ‘‘Standard (mm) .iam’ assembly’ and save it with the name ‘Chain-Inventor Studio’.
  50. Select ‘Place component’ tool from the marking menu and place the ‘Master’ Part in the Assembly.
  51. Select the ‘Master’ Sketch from the Browser Bar, right click and deselect Grounded from the context menu.
  52. Select the ‘Master’ Sketch again and make it ‘Adaptive’ from the context menu.
  53. Align the model in appropriate position using the View Cube.
  54. Apply a Flush Mate between YZ Plane of Assembly and YZ Plane of Master Sketch.
  55. Apply a Flush Mate between XZ Plane of Assembly and XZ Plane of Master Sketch.
  56. Apply a Flush Mate between XY Plane of Assembly and XY Plane of Master Sketch.
  57. Apply a Mate Constraint between YZ Plane of Assembly and Work Plane1 of Master Sketch.
  58. Inter the value 320mm in the Offset input box.
  59. Select ‘Place component’ tool from the marking menu and place the ‘Chain-Link’ part in the Assembly.
  60. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
  61. Apply a Mate Constraint between Centre Point of ‘Chain-Link’ and Work Point2 of Master Sketch.
  62. Change the view of design window by using View Cube.
  63. Align the Chain-Link in correct position by using Rotate Component Tool.
  64. Apply a Mate Constraint between XY Plane of Assembly and XZ Plane of ‘Chain-Link’.
  65. Apply Angle Constraint, between XZ Plane of Assembly and XY Plane of ‘Chain-Link’.
  66. Select Directed Angle option in the solution field.
  67. Now ‘Chain-Link’ is fully constrained in the Assembly.
  68. Start the Pattern Component Tool from the Component Panel of Assemble tab.
  69. Select the ‘Chain-Link’ as component, then select Rectangular Pattern2 of Master Sketch in the Browser Bar as Associative Feature Pattern.
  70. Click OK.
  71. Now all the ‘Chain-Links’ are fitted on the Curve loop.
  72. Close the visibility of Work Planes visible in the design window.
  73. Select ‘Place component’ from the marking menu and place the ‘Small-Sprocket’ in the Assembly.
  74. Create a Work Axis in the Assembly on this point, parallel to Z Axis of the Assembly.
  75. Apply a Mate Constraint between Axis of ‘Small-Sprocket’ and newly created Work Axis of the Assembly.
  76. Apply a Mate Constraint between XY Plane of Assembly and Mid Plane of the ‘Small-Sprocket’.
  77. Select ‘Place component’ from the marking menu and place the ‘Large-Sprocket’ in the Assembly.
  78. Apply a Mate Constraint between Axis of ‘Large-Sprocket’ and Z Axis of the Assembly.
  79. Apply a Mate Constraint between XY Plane of Assembly and Mid Plane of the ‘Large-Sprocket’.
  80. Change the view of design window by using View Cube.
  81. Activate Motion Constraint Command, first select Axis of ‘Large-Sprocket’ and then select Axis of ‘Small-Sprocket’. Click OK.
  82. Apply an Angle Constraint between XZ Plane of Assembly and YZ Plane of ‘Large-Sprocket’.
  83. Select Directed Angle option in the solution field.
  84. Change the name of Mate:1 constraint to ‘Drive-1’, and Angle:3 constraint to ‘Drive-2’ in the Browser Bar.
  85. Click the ‘Inventor Studio’ icon from the Begin Panel of Environments Tab.
  86. Select Drive-1 Constraint of Master Part in the Browser Bar, right click and select Animate Constraint in the context menu.
  87. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 30 second in the End input box.
  88. In ‘Action’ section, enter the value 1 mm in the End input box.
  89. Click Acceleration Tab.
  90. Select Constant Speed radio button in the Velocity Profile.
  91. Click OK.
  92. Select Expand Action Editor Button on the Animation Timeline.
  93. Select Drive-2 Angle Constraint of Large-Sprocket in the Browser Bar, right click and select Animate Constraint in the context menu.
  94. In the ‘Action’ section of Animate Constraint dialogue box, enter the value -360 degree in the End input box.
  95. In the ‘Time’ section, click the Specify Start Time button.
  96. Click Acceleration Tab.
  97. Select Constant Speed radio button in the Velocity Profile.
  98. Click OK.
  99. Select Collapse Action Editor Button on the Animation Timeline.
  100. Click the Animation Options Button.
  101. In the Animation Options dialogue box, select Constant Speed radio button in the Default Velocity Profile.
  102. Click Ok.
  103. Close the visibility of all the Sketches and Work features.
  104. Clear the screen by activating the Clean Screen command.
  105. Click ‘Go to Start’ Button.
  106. Click Play Animation button.
Note:-
13

 

Length of One Chain-Link 

Length of One Chain-Link

Loop length of Chain Profile


Loop length of Chain Profile
..................
Watch the following video to understand how to create the Link of the Chain.......



Dear viewers an advance version of Chain Animation tutorial showing the animation of 70 Chain Links along with 3 Sprockets can be seen on the following link…
Chain-Inventor Studio (Upgraded Design) - Autodesk Inventor 2013