Bottle Cap (Autodesk Inventor Tutorial 2013)

In this video viewer will be able to watch Basic Sketching features of Autodesk Inventor like; Circle, Arc, Circular Pattern . Other than this surface tools like Boundary Patch, Surface Loft, Sculpt are presented as well as Loop Fillet, Shell, Appearance Settings- lightening and half section view setting  are displayed. So watch the video and if you find interesting Like it and Share it.

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Bottle Cap (Deformation effect as after using an Opener)

This can be done by creating a line over the top of the model and using it as a base by Bend Tool.
 

Click the following link to get the model file: - http://bit.ly/2oP2XKl

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.

Pipe Wrench-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 182

Pipe Wrench-Dynamic Simulation-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 Dynamic Simulation of the ‘Pipe Wrench’.

 

Click the following link to get the model file: - http://bit.ly/2mT1v8y

 

Transcription of Video

Display of Motion in ‘Pipe Wrench’ through Dynamic Simulation.

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Pipe Wrench-Dynamic Simulation’.
2. Select Place component from the marking menu and place the ‘Base Frame’ 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. Place the ‘Supporting Bracket’ in the Assembly.
6. Apply an Axis Mate between hole on the Base Frame and hole on the Supporting Bracket.
7. Apply a Flush Mate Between XY Plane of Base Frame and XY Plane of Supporting Bracket.
8. Activate Angle Constraint Command first select side face of Base Frame; then select side face of Supporting Bracket and at the last select top face of Supporting Bracket.
9. Enter the value -4.76 degree in the Angle Input Box and click OK.
10. Place the ‘Rivet-1’ in the Assembly.
11. Fix the Rivet-1 in the hole of Supporting Bracket by the use of Insert Mate as displayed.
12. Place the ‘Supporting Strip-1’ in the Assembly.
13. Place the Supporting Strip -1 on the hole of Base Frame with the help of Insert Mate.
14. Apply an Angle Constraint between top face of Supporting Strip -1 and top face of Base Frame.
15. In the Solution Type, select Directed Angle.
16. Place the ‘Rivet-2’ in the Assembly.
17. Fix the Rivet-2 on the hole of Supporting Strip-1 with the help of Insert Mate.
18. Place the ‘Supporting Strip-2’ in the Assembly.
19. Place the Supporting Strip -2 on the hole of Base Frame with the help of Insert Mate.
20. Apply an Angle Constraint between top face of Supporting Strip -2 and top face of Base Frame.
21. In the Solution Type, select Directed Angle.
22. Drag the Rivet-2 from the Browser Bar in the Assembly. This will place a copy of Rivet-2 in the Assembly.
23. Fix the Rivet-2 on the hole of Supporting Strip-2 with the help of Insert Mate.
24. Place the ‘Sliding Frame’ in the Assembly.
25. Apply a Flush Mate between XY Plane of Base Frame and XY Plane of Sliding Frame.
26. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
27. Apply a Mate Constraint between X Axis of Sliding Frame and Work Plane 7 of Supporting Bracket.
28. Place the ‘Wheel’ in the Assembly.
29. Apply a Mate Constraint between X Axis of Sliding Frame and Axis of Wheel.
30. Apply a Mate Constraint between Work Plane 5 of Supporting Bracket and Work Plane 1 of Wheel.
31. Apply a Mate Constraint between Jaw of Base Frame and Jaw of Sliding Frame in the Assembly.
32. Select the previous applied ‘Mate: 5’ under the Constraints folder in the Browser Bar, Right click and choose ‘Supress’ from the context menu.
33. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
34. Select Insert Joint in the Marking menu.
35. Select ‘Screw’ from the drop down menu of Insert Joint dialog box.
36. In the Insert Joint dialog box, select Circular edge of Sliding Frame in ‘Component 1’ selection option and select Circular edge of Wheel in ‘Component 2’ selection option.
37. Enter the value 0.205 in the ‘Pitch’ input box. Click OK.
38. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
39. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
40. Click the arrow to expand the input choices, and click Constant Value.
41. Enter the value (-360/0.205) deg/s and click OK.
42. In Simulation Player, fill the value 1000 in the Images field area.
43. Clear the screen by activating the Clean Screen command.
44. Click Run in the Simulation Player to display motion in Pipe Wrench.

Pipe Wrench-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

  

Serial No. 75

Pipe Wrench-Drive Constraint-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 'Pipe Wrench’.

 

    

Click the following link to get the model file: - http://bit.ly/2njQE7E

Transcription of Video

Display of Motion in ‘Pipe Wrench’ through Drive Constraint.

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Pipe Wrench-Drive Constraint’.
2. Select Place component from the marking menu and place the ‘Base Frame’ 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. Place the ‘Supporting Bracket’ in the Assembly.
6. Apply an Axis Mate between hole on the Base Frame and hole on the Supporting Bracket.
7. Apply a Flush Mate Between XY Plane of Base Frame and XY Plane of Supporting Bracket.
8. Activate Angle Constraint Command first select side face of Base Frame; then select side face of Supporting Bracket and at the last select top face of Supporting Bracket.
9. Enter the value -4.76 degree in the Angle Input Box and click OK.
10. Place the ‘Rivet-1’ in the Assembly.
11. Fix the Rivet-1 in the hole of Supporting Bracket by the use of Insert Mate as displayed.
12. Place the ‘Supporting Strip-1’ in the Assembly.
13. Place the Supporting Strip -1 on the hole of Base Frame with the help of Insert Mate.
14. Apply an Angle Constraint between top face of Supporting Strip -1 and top face of Base Frame.
15. In the Solution Type, select Directed Angle.
16. Place the ‘Rivet-2’ in the Assembly.
17. Fix the Rivet-2 on the hole of Supporting Strip-1 with the help of Insert Mate.
18. Place the ‘Supporting Strip-2’ in the Assembly.
19. Place the Supporting Strip -2 on the hole of Base Frame with the help of Insert Mate.
20. Apply an Angle Constraint between top face of Supporting Strip -2 and top face of Base Frame.
21. In the Solution Type, select Directed Angle.
22. Drag the Rivet-2 from the Browser Bar in the Assembly. This will place a copy of Rivet-2 in the Assembly.
23. Fix the Rivet-2 on the hole of Supporting Strip-2 with the help of Insert Mate.
24. Place the ‘Sliding Frame’ in the Assembly.
25. Apply a Flush Mate between XY Plane of Base Frame and XY Plane of Sliding Frame.
26. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
27. Apply a Mate Constraint between X Axis of Sliding Frame and Work Plane 7 of Supporting Bracket.
28. Place the ‘Wheel’ in the Assembly.
29. Apply a Mate Constraint between X Axis of Sliding Frame and Axis of Wheel.
30. Apply a Mate Constraint between Work Plane 5 of Supporting Bracket and Work Plane 1 of Wheel.
31. Activate the Motion constraint, in the Type area select Rotation-Translation, and afterwards select the front face of Wheel then Vertical edge of Sliding Frame.
32. Enter the value 0.205 inch in the Distance Input box and click OK.
33. Activate the Angle Constraint, First select YZ Plane of Wheel, Second select XY Plane of Assembly and at last select top face of Supporting Bracket, and click OK.
34. Apply a Mate Constraint between Jaw of Base Frame and Jaw of Sliding Frame in the Assembly.
35. Select the previous applied ‘Mate: 5’ under the Constraints folder in the Browser Bar, Right click and choose ‘Supress’ from the context menu.
36. Select the Angle:4 Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
37. Right click the ‘Drive’ Constraint and select ‘Drive Constraint’ Tool from the context menu.
38. In the Drive Constraint dialog box, set the End value to (360/0.205).
39. Clear the screen by activating the Clean Screen command.
40. Click the Forward Button to display motion in ‘Pipe Wrench’.
41. To close the Jaw, click Reverse Button.

Hinge-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 49

Hinge-Autodesk Inventor 2012 (with caption and audio narration)

 

Click the following link to get the model file: - http://bit.ly/2lHZ1cO

 

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.

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.

Drill Machine-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

  

Serial No. 30

Drill Machine-Dynamic Simulation-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 Dynamic Simulation of the ‘Drill Machine’.

 

 

Click the following link to get the model file: -http://bit.ly/2ncLp9z

 

 

Transcription of Video

Display of Motion in Drill Machine through Dynamic Simulation

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Drill Machine-Dynamic Simulation’.
2. Select Place component from the marking menu and place the Frame in the Assembly.
3. Place Handle-1 and Handle Cap-1 in the Assembly.
4. Start the Constrain Command and choose Insert Mate from the type option.
5. First select the inner circular edge of Handle Cap, then select outer circular edge of Handle and click Ok.
6. Give another Insert Mate between Inner edge of Handle Cap and circular edge of Frame as displayed.
7. Re-orient the design window using View Cube.
8. Set the current view as Home View using the toggle next to View Cube.
9. Place Gear Wheel and Gear in the Assembly.
10. Apply a Mate Constraint between Axis of Gear Wheel and Axis of Gear.
11. Next, apply a Mate Constraint between face of Gear Wheel and face of Gear.
12. Apply another Mate Constraint between YZ Plane of Gear Wheel and XZ Plane of Gear.
13. Re-orient the Gear Wheel with respect to Frame using Rotate Component Tool.
14. Apply an Axis Mate between Gear Wheel and stud of Frame.
15. Place Spindle in the Assembly.
16. Apply a Mate Constraint between Axis of Frame and Axis of Spindle.
17. Next, apply a Mate Constraint between inner face of supporting cylinder of frame and back face of the spindle.
18. Place Pinion-2 in the Assembly.
19. Apply a Mate Constraint between Axis of Pinion-2 and Axis of Spindle.
20. Apply an Axis Mate between hole on Pinion-2 and hole on Spindle.
21. Place Locking Pin in the Assembly and fix it inside the hole of Pinion using Insert Mate.
22. Place Pinion-1 in the Assembly.
23. Align the Pinion-1 to match it with the Frame.
24. Apply a Mate Constraint between Axis of Frame and Axis of Pinion-1.
25. Select Pinion-1, Pinion-2 and Gear, then right click in the design window, choose ‘Isolate’ from the context menu.
26. Set the Browser from Assembly view to Modeling View.
27. Locate the Intersection Point of Pinion-2 inside the Browser Bar.
28. Apply a Mate Constraint between the Intersection Point of Pinion-2 and Intersection Point of Gear.
29. In the same manner, apply a Mate Constraint between the Intersection Point of Pinion-2 and the Intersection Point of Pinion-1.
30. Activate Motion Constraint; first select the Axis of Pinion-1 and afterward the Axis of Gear.
31. Enter the value 15/56 in the Ratio Input box and click Apply.
32. Apply same step as above to give motion constraint between Pinion-2 and Gear.
33. Right click in the design window, choose Undo Isolate from the context menu.
34. Place Chuck in the Assembly.
35. Apply a Mate Constraint between the Axis of Spindle and the Axis of Chuck.
36. Place a Mate Constraint between inner circular face of Chuck and front face of Spindle.
37. Place another Mate Constraint between YZ Plane of Chuck and YZ Plane of Spindle.
38. Place Three instances of Jaw in the Assembly.
39. Apply an Axis Mate between two subsequent Jaws.
40. Next, apply a Mate between their edges.
41. Apply a Flush Mate between their end faces.
42. In the same manner, constraint the third Jaw.
43. Apply a Mate Constraint between inner circular face of Chuck and rear face of Jaw.
44. Apply a Mate Constraint between the Axis of Chuck and the Axis of Jaw.
45. Place a Mate Constraint between YZ Plane of Chuck and YZ Plane of any one Jaw.
46. Place Handle-2 and Handle Cap-2 in the Assembly.
47. Apply an Insert Mate between inner circular edge of Handle Cap-2 and outer circular edge of Handle-2.
48. Position the Handle Cap-2 in respect of the stud of Frame by using Rotate Component Tool.
49. Apply an Insert Mate between front circular edge of Handle Cap-2 and inner circular edge of stud.
50. Place Handle Connecting Plate in the Assembly.
51. Apply an Insert Mate between edge of the hole on Handle Connecting Plate and inner circular edge of stud.
52. Place Washer-1 in the Assembly.
53. Apply an Insert Mate between edge of the hole on Washer-1 and edge of the hole on Gear Wheel.
54. Apply a Mate Constraint between YZ Plane of Handle Connecting Plate and Axis of the hole on Gear Wheel.
55. Place Screw-2 in the Assembly.
56. Apply an Insert Mate between inner circular edge of Screw-2 and edge of the hole on Handle Connecting Plate.
57. Place Handle-3 and Handle Cap-3 in the Assembly.
58. Fit the Handle Cap-3 over the Handle-3 with the help of Insert Mate.
59. Apply another Insert Mate between the Handle Cap-3 and hole on the Handle Connecting Plate.
60. Place Screw-1 and Nut in the Assembly.
61. Fix the Screw-1 on the Handle-3 with the help of Insert Mate.
62. Fix the Nut on the Screw-1 by applying Insert Mate.
63. Open the Visibility of surfaces named ‘Pitch Diameter’ of Pinion-2, Pinion-1 and Gear.
64. ‘Isolate’ the Pinion-1, Pinion-2 and Gear in the Assembly.
65. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
66. Select Insert Joint in the Marking menu.
67. Select ‘Rolling: Cone on Cone’ from the drop down menu of Insert Joint dialog box.
68. Select Pitch Diameter of Pinion-2 in ‘Component 1’ option and select Pitch diameter of Gear in ‘Component 2’ option and click Apply.
69. In the same manner select Pitch Diameter of Pinion-1 and select Pitch diameter of Gear and click Ok.
70. Finish Dynamic Simulation and return to Assembly Modelling environment.
71. Close the visibility of surfaces named ‘Pitch Diameter’ of Pinion-1, Pinion-2 and Gear.
72. Right Click in the design window and click ‘Undo Isolate’ option.
73. Activate Dynamic Simulation Tool.
74. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
75. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
76. Click the arrow to expand the input choices, and click Constant Value.
77. Enter the value 360 deg/s and click Ok.
78. In Simulation Player, fill the value 1000 in the Images field area.
79. Clear the screen by activating the Clean Screen command.
80. Click Run in the Simulation Player to display motion in Drill Machine.

Vise-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 106

Vise-Dynamic Simulation-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 Dynamic Simulation of the ‘Vise’.

 

Click the following link to get the model file: - http://bit.ly/2ms77GX

 

 

 Transcription of Video

Display of Motion in Vise through Dynamic Simulation

Sub Assembly-1:

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Sub Assembly-1’.
2. Select Place component from the marking menu and place the ‘Base Housing’ 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. Place the ‘Part-1’ in the Assembly.
6. Apply a Mate Constraint between the bottom face of Part-1 and inner face of Base Housing.
7. Apply another Mate Constraint between YZ plane of Base Housing and YZ Plane of Part-1.
8. Apply a Flush Mate between front face of Part-1 and front face of Base Housing.
9. Fill the offset value 5.672 inch.
10. Place the ‘Jaw Plate’ in the assembly.
11. Apply a Mate Constraint between slotted face of Base Housing and back face of Jaw Plate.
12. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate.
13. Apply a Flush Mate between the side face of Jaw Plate and side face of Base Housing.
14. Place two identical ‘Screws’ in the Assembly.
15. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate.
16. Save the Sub Assembly-1 and close it.

Sub Assembly-2:

1. Create a New Assembly and save it with the name ‘Sub Assembly-2’.
2. Select Place component from the marking menu and place the ‘Sliding Housing’ 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. Place the ‘Jaw Plate’ in the Assembly.
6. Apply a Mate Constraint between slotted face of Sliding Housing and back face of Jaw Plate.
7. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate.
8. Apply a Flush Mate between the side face of Jaw Plate and side face of Sliding Housing.
9. Place two identical ‘Screws’ in the Assembly.
10. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate.
11. Save the Sub Assembly-2 and close it.

Sub Assembly-3:

1. Create a New Assembly and save it with the name ‘Sub Assembly-3’.
2. Select Place component from the marking menu and place the ‘Threaded Spindle’ in the Assembly.
3. Place the ‘Compress Spring’ in the Assembly.
4. Apply a Mate Constraint between Y Axis of Compress Spring and Axis of Threaded Spindle.
5. Apply a Mate Constraint between circular face of Threaded Spindle and face of Compress Spring.
6. Place the ‘Washer’ in the Assembly.
7. Apply an Axis Mate between Washer and Threaded Spindle.
8. Apply a Mate Constraint between face of Washer and face of Compress Spring.
9. Place the ‘Pin’ in the Assembly.
10. Apply an Axis Mate between Pin and hole on the Threaded Spindle.
11. Apply a Mate Constraint between XY Plane of Threaded Spindle and YZ Plane of Pin.
12. Place the ‘Handle’ in the Assembly.
13. Apply an Axis Mate between hole on the Threaded Spindle and Handle.
14. Next apply a Mate Constraint between XZ plane of Threaded Spindle and YZ Plane of Handle.
15. Save the Sub Assembly-3 and close it.

Main Assembly (Vise):

1. Create a New Assembly and save it with the name ‘Vise-Dynamic Simulation’.
2. Select Place component from the marking menu and place the ‘Sub Assembly-1’ 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. Place ‘Sub Assembly-2’ in the Assembly.
6. Align the Sub Assembly-2 in front of Sub Assembly-1 by using Rotate Component Tool.
7. Apply a Mate Constraint between the bed of Sub Assembly-1 and bottom face of Sub Assembly-2.
8. Apply a Flush Mate between YZ Plane of Sub Assembly-1 and XY Plane of Sub Assembly-2.
9. Place ‘Sub Assembly-3’ in the Assembly.
10. Apply an Axis Mate between hole on the Sliding Housing and Threaded Spindle.
11. Apply a Mate Constraint between outer rim of hole on Sliding Housing and rear face of Threaded Spindle.
12. Apply a Mate Constraint between subsequent faces of Jaw in the Assembly.
13. Select the previous applied ‘Mate:4’under the Sub Assembly-1 in the Browser Bar, Right click and choose ‘Supress’ from the context menu.
14. Dynamic Simulation
15. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
16. Select Insert Joint in the Marking menu.
17. Select ‘Screw’ from the drop down menu of Insert Joint dialog box.
18. In the Insert Joint dialog box, select Circular edge of Threaded Spindle in ‘Component 1’ selection option and select Circular edge of Part-1 in ‘Component 2’ selection option.
19. Enter the value 1/7 in the ‘Pitch’ input box. Click OK.
20. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
21. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
22. Click the arrow to expand the input choices, and click Constant Value.
23. Enter the value -360*7 deg/s and click OK.
24. In Simulation Player, fill the value 1000 in the Images field area.
25. Clear the screen by activating the Clean Screen command.
26. Click Run in the Simulation Player to display motion in Vise.
27. Change the colour of Vise ‘Green (Clear)’ to watch its motion in transparent view.

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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Bolt-Nut-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 8

Bolt-Nut-Dynamic Simulation-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 Dynamic Simulation of the ‘Bolt and Nut’.

 

Click the following link to get the model file:- http://bit.ly/2n9ebrD

Roller Chain-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 81

Roller Chain-Dynamic Simulation-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 Dynamic Simulation of  the ‘Roller Chain’.

 

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

 

Transcription of Video

Display motion in Roller Chain through Dynamic Simulation.

1. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘Roller Chain–Dynamic Simulation’.
2. Hold the Ctrl key, and click the Roller Chains tool on the Power Transmission panel of the Design tab.
3. The Roller Chains Generator dialog box will open with its default values.
4. At present ‘Select Chain Mid Plane’ selection is active by default.
5. Select XY Plane of the Assembly.
6. Select first Roller Chain Sprocket 1 pulley in the ‘Sprockets’ section. Click Sprocket properties button to change the sprocket parameters.
7. Enter the value 38 in the ‘Teeth’ input box and click OK.
8. Click OK again.
9. Align the Roller Chain in correct position by using View Cube.
10. Change the color of both the Sprockets from the Browser Bar to watch it more clearly.
11. Select the ‘Chain Drive’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu.
12. Now both the Sprockets are rotating on their own Axis.
13. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
14. Activate Insert Joint from the Marking menu.
15. Select ‘Belt’ from the drop down menu of Insert Joint dialog box.
16. In the Insert Joint dialog box, select edge of small Sprocket as ‘Component 1’ and select edge of large Sprocket as ‘Component 2’. Click Ok.
17. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
18. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
19. Click the arrow to expand the input choices, and click Constant Value.
20. Enter the value 360*3 deg/s and click Ok.
21. In Simulation Player, fill the value 2000 in the Images field area.
22. Clear the screen by activating the Clean Screen command.
23. Click Run in the Simulation Player to display motion in Roller Chain.

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

Serial No.  93

Synchronous Belt-Dynamic Simulation-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 Dynamic Simulation of the ‘Synchronous Belt’.

 

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

 

Transcription of Video

Display motion in Synchronous Belt through Dynamic Simulation.

1. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘Synchronous Belt–Dynamic Simulation’.
2. Hold the Ctrl key, and click the Synchronous Belts tool on the Power Transmission panel of the Design tab.
3. The Synchronous Belts Component Generator dialog box will open with its default values.
4. At present ‘Belt Mid Plane’ selection is active by default.
5. Select XY Plane of the Assembly.
6. Select first Synchronous pulley in the ‘Pulleys’ section. Click Pulley properties button to change the pulley parameters.
7. Enter the value 38 in the ‘Teeth’ input box and click OK.
8. Select Second Synchronous pulley in the ‘Pulleys’ section. Click Pulley properties button.
9. Enter the value 57 in the ‘Teeth’ input box and click OK.
10. Click OK again.
11. Align the Belt in correct position by using View Cube.
12. Change the colour of both the Pulleys from the Browser Bar to watch it more clearly.
13. Select the ‘Synchronous Belts Transmission’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu.
14. Now both the Pulleys are rotating on their own Axis.
15. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
16. Activate Insert Joint from the Marking menu.
17. Select ‘Belt’ from the drop down menu of Insert Joint dialog box.
18. In the Insert Joint dialog box, select edge of small Pulley as ‘Component 1’ and select edge of large Pulley as ‘Component 2’. Click Ok.
19. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
20. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
21. Click the arrow to expand the input choices, and click Constant Value.
22. Enter the value 360*3 deg/s and click Ok.
23. In Simulation Player, fill the value 2000 in the Images field area.
24. Clear the screen by activating the Clean Screen command.
25. Click Run in the Simulation Player to display motion in Synchronous Belt.

V-Belt-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 103

V-Belt-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to give the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘V-Belt’.

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

 

Transcription of Video

Display motion in V-Belt through Dynamic Simulation.

1. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘V-Belt–Dynamic Simulation’.
2. Hold the Ctrl key, and click the V-Belts tool on the Power Transmission panel of the Design tab.
3. The V-Belts Component Generator dialog box will open with its default values.
4. At present ‘Belt Mid Plane’ selection is active by default.
5. Select XY Plane of the Assembly.
6. Select Second Grooved Pulley in the ‘Pulleys’ section. Click Pulley properties button to change the pulley parameters.
7. In ‘Design Guide’ drop down menu, select Transmission Ratio.
8. Enter the value 1.5 in the Ratio input box. Click OK.
9. Click OK again.
10. Align the Belt in correct position by using View Cube.
11. Change the colour of both the Pulleys from the Browser Bar to watch it more clearly.
12. Select the ‘V-Belts transmission’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu.
13. Now both the Pulleys are rotating on their own Axis.
14. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
15. Activate Insert Joint from the Marking menu.
16. Select ‘Belt’ from the drop down menu of Insert Joint dialog box.
17. In the Insert Joint dialog box, select edge of small Pulley as ‘Component 1’ and select edge of large Pulley as ‘Component 2’. Click Ok.
18. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
19. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
20. Click the arrow to expand the input choices, and click Constant Value.
21. Enter the value 360*3 deg/s and click Ok
22. In Simulation Player, fill the value 1000 in the Images field area.
23. Clear the screen by activating the Clean Screen command.
24. Click Run in the Simulation Player to display motion in V-Belt Belt.

Worm Gear-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 109

Worm Gear-Dynamic Simulation-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 Dynamic Simulation of the ‘Worm Gear’.

 

 

Click the following link to get the model file: - http://bit.ly/2mAv1zO

 

 

 

Transcription of Video

Display motion in Worm Gear through Dynamic Simulation

1. Create a ‘New Assembly’ and save it with the name ‘Worm Gear–Dynamic Simulation’.
2. Select Place component from the marking menu and place the Worm in the Assembly.
3. Select the Worm in the Design window, right click and deselect Grounded from the context menu.
4. At present there are six Degrees of Freedom in Worm and it can be moved in any direction in the Assembly.
5. Open the visibility of X Axis of Assembly and X Axis of Worm from the Browser Bar and then apply a Mate Constraint between them.
6. Apply another Mate Constraint between Centre Point of the Assembly and Centre Point of the Worm.
7. Now only one Degree of Freedom is left and Worm can be moved only on its X Axis.
8. Select Place component from the marking menu and place the Worm Gear in the Assembly.
9. Align the Worm Gear in correct position by using Rotate Component Tool.
10. Open the visibility of XZ Plane of Assembly and XY Plane of Worm Gear from the Browser Bar and then apply a Mate Constraint between them.
11. Close the visibility of Work Planes to clear the screen.
12. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
13. Open the visibility of Pitch Diameter of Worm Gear and Pitch Diameter of Worm and then apply a Tangent Mate between them.
14. Apply another Mate Constraint between the Z Axis of Worm Gear and YZ Plane of Assembly.
15. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Worm Gear.
16. Activate the Work Axis command from the Work Features Panel of Assemble Tab, and then select Through Revolved Face or Feature in the Axis drop down menu.
17. Select Pitch Diameter of Worm Gear to create the Work Axis.
18. In the Quick Access toolbar, click the selection tool dropdown list and choose Select Sketch Features.
19. Convert this Work Axis to ‘Grounded’.
20. Activate the Motion Constraint, first select the side face of Worm and then the top face of Worm Gear. In the Ratio input box, enter the value 1/40 and click Ok.
21. Once again, check the Degrees of Freedom of Worm Gear and Worm in the assembly, this time both the gears are rotating on their own Axis.
22. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
23. Activate Insert Joint from the Marking menu.
24. Select ‘Worm Gear’ from the drop down menu of Insert Joint dialog box.
25. In the Insert Joint dialog box, select Pitch Diameter of Worm in ‘Gear option’ and select Pitch Diameter of Worm Gear in ‘Screw option’. Enter the value (- 1/40 ) in the Pitch input box. Click Ok.
26. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
27. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
28. Click the arrow to expand the input choices, and click Constant Value.
29. Enter the value 360*40 deg/s and click Ok.
30. Close the visibility of Pitch diameter of Worm Gear and Worm.
31. In Simulation Player, fill the value 1000 in the Images field area.
32. Clear the screen by activating the Clean Screen command.
33. Click Run in the Simulation Player to display motion in Worm and Worm Gear.

Note: - The worm gear is always driven by the worm.

Helical Gear-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 48

Helical Gear-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to give the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Helical Gear’.

 

 

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

 

 

 Transcription of Video

Display motion in Helical Gear through Dynamic Simulation

1. Create a ‘New Assembly’ and save it with the name ‘Helical Gear–Dynamic Simulation’.
2. Select Place component from the marking menu and place the Helical Gear in the Assembly.
3. Align the Gear in correct position by using View Cube.
4. Select the Gear in the Design window, right click and deselect Grounded from the context menu.
5. At present there are six Degrees of Freedom in Gear and it can be moved in any direction in the Assembly.
6. Open the visibility of Z Axis of Assembly and Z Axis of Gear from the Browser Bar, and then apply a Mate Constraint between them.
7. Apply another Mate Constraint between Centre point of the Assembly and Centre point of the Gear.
8. Now this time only one Degrees of Freedom is left and Gear can be moved only on its Z Axis.
9. Select Place component from the marking menu and place the Pinion in the Assembly.
10. Activate the Constraint command and change the constraint type to Flush in the Solution field, select the top face of Pinion and top face of Gear, click apply.
11. Apply a Mate Constraint between YZ Plane of Gear and YZ Plane of Pinion.
12. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
13. Open visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion and then apply a Tangent Mate between them.
14. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Pinion.
15. Activate the Work Axis command from the Work Features Panel of Assemble Tab, and then select Through Revolved Face or Feature in the Axis drop down menu.
16. Select Pitch Diameter of Pinion to create the Work Axis.
17. In the Quick Access toolbar, click the selection tool dropdown list and choose Select Sketch Features.
18. Convert this Work Axis to ‘Grounded’.
19. Activate the Motion Constraint, first select the top face of Pinion and then top face of Gear. In the Ratio input box, enter the value 23/57 and click Ok.
20. Suppress the Mate:3 Constraint in the Browser.
21. Once again, check the Degrees of Freedom of gear and pinion in the assembly, this time both the gears are rotating on their own Axis.
22. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
23. Select Insert Joint in the Marking menu.
24. Select ‘Rolling: Cylinder on Cylinder’ from the drop down menu of Insert Joint dialog box.
25. Select Rolling constraint option.
26. First select the Pitch Diameter of Pinion and then the Pitch Diameter of Gear. Click Ok.
27. Select Revolution:3 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
28. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
29. Click the arrow to expand the input choices, and click Constant Value.
30. Enter the value 360.000 deg/s, and click Ok.
31. In the Images field, enter the value 1000.
32. Close the visibility of Pitch diameter of Helical Gear and Pinion.
33. Mesh the teeth of Gear and Pinion manually in front of each other, after Suppressing the Motion Constraint.
34. Once again Un-suppress the Motion Constraint.
35. Clear the screen by activating the Clean Screen command.
36. Click Run in the Simulation Player to display motion in Helical Gear and Pinion.