Chain-Inventor Studio (Upgraded Design) - Autodesk Inventor 2013

Serial No. 220

Chain-Inventor Studio (Upgraded Design) - Autodesk Inventor 2013

This video displays a setting up of 70 chain links and 3 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……

 

Click the following link to get the model file: -http://bit.ly/2nIJIRH

Synchronous Belt-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 94

Synchronous Belt-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation of the ‘Synchronous Belt’.

 

Click the following link to get the model file: - http://bit.ly/2mC9Z3Z

 

Transcription of Video

Display of motion in ‘Synchronous Belt-Inventor Studio’ through Inventor Studio

1. Create a New ‘Standard (mm) .ipt’ Part file.
2. At present Sketch1 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. Create a new Work Plane Parallel to YZ Plane at an offset distance of 323.623 mm.
6. Create a new Sketch on XY Plane.
7. Draw a Circle of 97.021 mm diameter, coincident with the auto projected part origin.
8. Create another Circle of 72.766 mm diameter. The distance between these two circles is 323.623 mm.
9. Take the project of X Axis and convert it to construction geometry.
10. The centre of small circle is 12.128 mm below the projected X Axis line.
11. Draw a line connecting top of two circles as displayed.
12. Take the project of YZ Plane and convert it to construction geometry.
13. Draw another line between two circles.
14. Erase the unwanted sketches by using the Trim tool.
15. Apply dimensions to fully constraint the sketch as displayed.
16. Take the project of Work Plane1 from the browser bar, with use of Project Geometry tool.
17. Convert this line into construction geometry.
18. Apply a dimension between these two projected lines. This dimension is driven dimension.
19. Now the sketch is complete, exit the sketch environment.
20. Create a Work Point at the intersection of YZ Plane and bottom line of the sketch.
21. Activate the Parameters tool from the Parameters Panel of the Manage tab.
22. Create a User defined Parameter named ‘start’ by clicking ‘Add Numeric’ button in the Parameters dialog box.
23. Click the ‘Equation’ column and then select the driven dimension in the design window.
24. Click Done.
25. Save the Part file with the name ‘Locus of Tooth’.
26. Start the Rectangular Pattern Tool and select Work Point1 in the Browser Bar as feature.
27. Click the ‘Direction 1’ button and select the sketch in the design window.
28. In the Column spacing input box, click arrow button to expand choices.
29. Select List Parameters then select the ‘start’.
30. Click more button to expand the dialogue box.
31. Select Adjust in the ‘Compute’ option.
32. Click the Start button in the ‘Direction 1’ field and select the Work Point1 in the Browser Bar.
33. Click OK.
34. Open the visibility of Sketch2 from the Browser Bar.
35. Select Work Plane1 in the Browser Bar and make it ‘Adaptive’ from the context menu.
36. Activate Rectangular Pattern Tool once again.
37. Select Work Point2 in the Browser Bar as feature.
38. Click the ‘Direction 1’ button and select the sketch in the design window.
39. In the Column Count input box, enter the value 72.
40. Click this drop down to specify pattern length.
41. Select ‘Curve Length’ option.
42. Click the more button to expand the dialogue box.
43. Select Adjust in the ‘Compute’ option.
44. Click the Start button in the ‘Direction 1’ field and select the Work Point2.
45. Select Direction1 in the ‘Orientation’ option.
46. Click OK.
47. Save the file and close it.
48. Create a ‘‘Standard (mm) .iam’ assembly’ and save it with the name ‘Synchronous Belt -Inventor Studio’.
49. Select ‘Place component’ tool from the marking menu and place the ‘Locus of Tooth’ Part in the Assembly.
50. Select the ‘Locus of Tooth’ Sketch from the Browser Bar, right click and deselect Grounded from the context menu.
51. Select the ‘Locus of Tooth’ Sketch again and make it ‘Adaptive’ from the context menu.
52. Align the model in appropriate position using the View Cube.
53. Apply a Flush Mate between YZ Plane of Assembly and YZ Plane of Locus of Tooth.
54. Apply a Flush Mate between XZ Plane of Assembly and XZ Plane of Locus of Tooth.
55. Apply a Flush Mate between XY Plane of Assembly and XY Plane of Locus of Tooth.
56. Apply a Mate Constraint between YZ Plane of Assembly and Work Plane1 of Locus of Tooth.
57. Inter the value 323.623 mm in the Offset input box.
58. Click OK.
59. Select ‘Place component’ tool from the marking menu and place the ‘Tooth’ 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 Work Point2 of ‘Tooth’ and Work Point2 of ‘Locus of Tooth’.
62. Change the view of design window by using View Cube.
63. Apply a Flush Mate between XY Plane of Assembly and XY Plane of ‘Tooth’.
64. Apply an Angle Constraint between XZ Plane of Assembly and XZ Plane of ‘Tooth’.
65. Select Directed Angle option in the solution field.
66. Close the visibility of Work Planes, visible in the design window.
67. Create a Work Axis in the Assembly on this point, parallel to Z Axis of the Assembly.
68. Place the ‘Belt-Base’ in the Assembly.
69. Apply a Mate Constraint between Z Axis of Assembly and Z Axis of Belt-Base.
70. Apply an Axis Mate between Belt-Base and Work Axis1 of Assembly.
71. Apply a Mate Constraint between XY Plane of Assembly and XY Plane of Belt-Base.
72. Start the Pattern Component Tool from the Component Panel of Assemble tab.
73. Select the ‘Tooth’ as component, then select Rectangular Pattern2 of Locus of Tooth in the Browser Bar as Associative Feature Pattern.
74. Click OK.
75. Now all the ‘Teeth’ are fitted on the Locus of Teeth.
76. Select ‘Place component’ from the marking menu and place the ‘Small Pulley’ in the Assembly.
77. Apply a Mate Constraint between Z Axis of ‘Small Pulley’ and Work Axis1 of the Assembly.
78. Apply a Mate Constraint between XY Plane of ‘Small Pulley’ and XY Plane of the Assembly.
79. Select ‘Place component’ from the marking menu and place the ‘Large Pulley’ in the Assembly.
80. Apply a Mate Constraint between Z Axis of ‘Large Pulley’ and Z Axis of the Assembly.
81. Apply a Mate Constraint between XY Plane of Assembly and XY Plane of the ‘Large Pulley’.
82. Change the view of design window by using View Cube.
83. Activate Motion Constraint Command, first select Z Axis of ‘Large Pulley’ and then select Z Axis of ‘Small- Pulley’. Click OK.
84. Apply an Angle Constraint between XZ Plane of Assembly and XZ Plane of ‘Small Pulley’.
85. Select Directed Angle option in the solution field.
86. Change the name of Mate:1 constraint to ‘Drive-1’, and Angle:3 constraint to ‘Drive-2’ in the Browser Bar.
87. Click the ‘Inventor Studio’ icon from the Begin Panel of Environments Tab.
88. Select Drive-1 Constraint of Locus of Tooth in the Browser Bar, right click and select Animate Constraints in the context menu.
89. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 30 second in the End input box.
90. In ‘Action’ section, enter the value 1 mm in the End input box.
91. Click Acceleration Tab.
92. Select Constant Speed radio button in the Velocity Profile.
93. Click OK.
94. Select Expand Action Editor Button on the Animation Timeline.
95. Select Drive-2 Angle Constraint of Small-Pulley in the Browser Bar, right click and select Animate Constraints in the context menu.
96. In the ‘Action’ section of Animate Constraint dialogue box, enter the value (-360 degree) in the End input box.
97. In the ‘Time’ section, click the Specify Start Time button.
98. Click Acceleration Tab.
99. Select Constant Speed radio button in the Velocity Profile.
100. Click OK.
101. Select Collapse Action Editor Button on the Animation Timeline.
102. Click the Animation Options Button.
103. In the Animation Options dialogue box, select Constant Speed radio button in the Default Velocity Profile.
104. Click Ok.
105. Close the visibility of all the Sketches and Work features.
106. Clear the screen by activating the Clean Screen command.
107. Click ‘Go to Start’ Button.
108. Click Play Animation button.

Nose Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 66

Nose Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation of the ‘Nose Pliers’.

 

Click the following link to get the model file: - http://bit.ly/2mgIw7T

 

Transcription of Video

Display of motion in ‘Nose Pliers’ through Inventor Studio

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Nose Pliers-Inventor Studio’.
2. Select Place component from the marking menu and place the ‘Part1’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Select the Part1 in the design window and remove its ‘Grounded’ position from the context menu.
6. Apply an Axis Mate between Z Axis of Assembly and hole of Part1.
7. Apply a Mate Constraint between XY Plane of Assembly and slotted face of Part1.
8. Place the ‘Part2’ in the Assembly.
9. Select the edge of small hole on Part2 to activate Assemble Tool.
10. Then select the edge of small hole on Part1, click green check mark to place Insert Mate between Part2 and Part1.
11. Activate an Angle Constraint, first Select face of Jaw of Part1, and then select YZ Plane of Assembly and in the end select top face of Part1. Click OK.
12. Activate Angle Constraint once again, first Select face of Jaw of Part2, and then select YZ Plane of Assembly and in the end select top face of Part2.
13. Enter the value 180 degree in the Angle Input box and Click Ok.
14. Place the ‘Rivet’ in the Assembly.
15. Select the inner circular edge of Rivet to activate Assemble Tool.
16. Then select the inner small circular edge of hole on the Part2, click green check mark to place Insert Mate between Part2 and Rivet.
17. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
18. Select ‘Angle:2’ constraint under the Constraints folder in the Browser Bar, Right click and choose ‘Suppress’ from the context menu.
19. Select Part1 and Part2 in the Browser Bar, right click and choose ‘Contact Set’ from the context menu.
20. Select ‘Activate Contact Solver’ in the Interference panel of Inspect Tab.
21. Drag the Part2, it will stop at the point of Collision between Part1 and Part2.
22. Measure the swing angle between the jaw of Part1 and Part2. The detected swing angle is 70.64 degree.
23. Restore the settings to previous state.
24. Click the ‘Inventor Studio’ icon from the Begin Panel of Environments Tab.
25. Select ‘Angle:1’ Constraint under Part1 in the Browser Bar, right click and select Animate Constraints in the context menu.
26. In ‘Action’ section of Animate Constraints dialogue box, enter the value 35.32 degree in the End input box.
27. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box.
28. Click Acceleration Tab.
29. Select ‘Constant Speed’ radio button in the Velocity Profile.
30. Click OK.
31. Select Expand Action Editor Button on the Animation Timeline.
32. Select Angle:1 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu.
33. Edit Mirrored animation action in the Animation Timeline.
34. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box, to give effect of 3 second pause.
35. Click OK.
36. Select ‘Angle:2’ Constraint under Part2 in the Browser Bar, right click and select Animate Constraints in the context menu.
37. In ‘Action’ section, enter the value (180-35.32) degree in the End input box.
38. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box.
39. Click Acceleration Tab.
40. Select ‘Constant Speed’ radio button in the Velocity Profile.
41. Click OK.
42. Select Angle:2 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu.
43. Edit Mirrored animation action in the Animation Timeline.
44. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box.
45. Click OK.
46. Select Collapse Action Editor Button on the Animation Timeline.
47. Click the Animation Options Button.
48. In the Animation Options dialogue box, click ‘Fit to Current Animation’ button in the ‘Length’ section option.
49. Select Constant Speed radio button in the Default Velocity Profile and click Ok.
50. Clear the screen by activating the Clean Screen command.
51. Click ‘Go to Start’ Button.
52. Click Play Animation button to display motion in Nose Pliers.

Combination Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 22

Combination Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation of the ‘Combination Pliers’.

 

  

Click the following link to get the model file: -http://bit.ly/2n4Yhig

 

Transcription of Video

Display of motion in ‘Combination Pliers’ through Inventor Studio

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Combination Pliers-Inventor Studio’.
2. Select Place component from the marking menu and place the ‘Part1’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Select the Part1 in the design window and remove its ‘Grounded’ position from the context menu.
6. Apply an Axis Mate between Z Axis of Assembly and Z Axis of Part1.
7. Apply a Mate Constraint between Centre Point of Assembly and Centre Point of Part1.
8. Place the ‘Part2’ in the Assembly.
9. Select the edge of small hole on Part2 to activate Assemble Tool.
10. Then select the edge of small hole on Part1, click green check mark to place Insert Mate between Part2 and Part1.
11. Activate an Angle Constraint, first Select face of Jaw of Part1, and then select YZ Plane of Assembly and in the end select top face of Part1. Click OK.
12. Activate Angle Constraint once again, first Select face of Jaw of Part2, and then select YZ Plane of Assembly and in the end select top face of Part2.
13. Enter the value 180 degree in the Angle Input box and Click Ok.
14. Place the ‘Rivet’ in the Assembly.
15. Select the inner circular edge of Rivet to activate Assemble Tool.
16. Then select the inner small circular edge of hole on the Part2, click green check mark to place Insert Mate between Part2 and Rivet.
17. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
18. Select ‘Angle:2’ under the Constraints folder in the Browser Bar, Right click and choose ‘Suppress’ from the context menu.
19. Select Part1 and Part2 in the Browser Bar, right click and choose ‘Contact Set’ from the context menu.
20. Select ‘Activate Contact Solver’ in the Interference panel of Inspect Tab.
21. Drag the Part2, it will stop at the point of Collision between Part1 and Part2.
22. Measure the swing angle between the jaw of Part1 and Part2. The detected swing angle is 40.18 degree.
23. Restore the settings to previous state.
24. Click the ‘Inventor Studio’ icon from the Begin Panel of Environments Tab.
25. Select ‘Angle:1’ Constraint under Part1 in the Browser Bar, right click and select Animate Constraints in the context menu.
26. In ‘Action’ section, enter the value -20.09 degree in the End input box.
27. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box.
28. Click Acceleration Tab.
29. Select ‘Constant Speed’ radio button in the Velocity Profile.
30. Click OK.
31. Select Expand Action Editor Button on the Animation Timeline.
32. Select Angle:1 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu.
33. Edit Mirrored animation action in the Animation Timeline.
34. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box, to give effect of 3 second pause.
35. Click OK.
36. Select ‘Angle:2’ Constraint under Part2 in the Browser Bar, right click and select Animate Constraints in the context menu.
37. In ‘Action’ section, enter the value (180+20.09) degree in the End input box.
38. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box.
39. Click Acceleration Tab.
40. Select ‘Constant Speed’ radio button in the Velocity Profile.
41. Click OK.
42. Select Angle:2 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu.
43. Edit Mirrored animation action in the Animation Timeline.
44. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box.
45. Click OK.
46. Select Collapse Action Editor Button on the Animation Timeline.
47. Click the Animation Options Button.
48. In the Animation Options dialogue box, click ‘Fit to Current Animation’ button in the ‘Length’ section option.
49. Select Constant Speed radio button in the Default Velocity Profile and click Ok.
50. Clear the screen by activating the Clean Screen command.
51. Click ‘Go to Start’ Button.
52. Click Play Animation button to display motion in Combination Pliers.

Chain-Inventor Studio-Autodesk Inventor 2013 (with caption and audio narration)

Serial N0. 17

In this Autodesk Inventor tutorial, we will learn how to create an animation of chain links similar to what we see in the real world. For this, we will use a chain link (total 61 after duplicating it by using Assembly components pattern tool ) and two sprockets.
While creating the animation we will use as well learn various tools and functionalities of the software like basic sketching, creating user-defined work planes and points, utilization of adaptivity features, application of pattern feature along with detailed settings, Assembly Mates, Inventor Studio etc.

Video:--

Click the following link to get the model file: - http://bit.ly/2n7CS7Q

 

 

 

Length of One Chain-Link 

Loop length of Chain Profile

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Related Blog Post

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

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