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.

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

Serial No. 181

Rack and Pinion-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 ‘Rack and Pinion’.

 

 

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

 

 

 

Transcription of Video

Display motion in Rack and Pinion through Dynamic Simulation.

1. Create a ‘New Assembly’ and save it with the name ‘Rack and Pinion-Dynamic Simulation’.
2. Select Place component from the marking menu and place the Pinion in the Assembly.
3. Align the Pinion in correct position by using View Cube.
4. Select the Pinion in the design window, right click and deselect Grounded from the context menu.
5. Open the visibility of Z Axis of Assembly and Z Axis of Pinion from the Browser Bar.
6. Apply a Mate Constraint between Z Axis of Assembly and Z Axis of Pinion.
7. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Pinion.
8. Place the Rack in the Assembly and align it properly with Pinion by using Rotate Component Tool.
9. Apply a Tangent Mate between Pitch Circle of Pinion and Pitch Line of Rack.
10. Activate Angle Constraint, First select XZ Plane of Assembly, Second select XZ Plane of Rack and in the Third select front face of Rack, and click OK.
11. Create a Work Plane in the assembly, coplanar with the base of Rack.
12. Convert this Work Plane to ‘Grounded’ in the Browser Bar.
13. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
14. Select Angle:1 Constraint in the Browser under the Constraints folder and Suppress it from the context menu.
15. Open the visibility of YZ Plane of Pinion and Work Plane 7 of Rack; later apply a mate constraint between them.
16. Turn off the visibility of Work Planes to make the screen clear.
17. Right click the Mate:6 in the browser and select Supress from the context menu.
18. Activate the Motion constraint, in the Type area select Rotation-Translation, and afterwards select the Pitch Circle of Pinion then Pitch Line of Rack. Fill the value 4.725 inch in the Distance Input box and click OK.
19. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
20. Select Insert Joint in the Marking menu.
21. Select ‘Rolling: Cylinder on Plane’ from the drop down menu of Insert Joint dialog box.
22. Select Rolling constraint option.
23. In the Insert Joint dialog box, select Pitch Line of Rack in ‘Plane’ option and select Pitch Circle of Pinion in ‘Cylinder’ option. Click Ok.
24. Select Revolution:1 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
25. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
26. Click the arrow to expand the input choices, and click Constant Value.
27. Enter the value (-575) deg/s and click Ok.
28. In Simulation Player, fill the value 1000 in the Images field area.
29. Clear the screen by activating the Clean Screen command.
30. Click Run in the Simulation Player to display motion in Rack and Pinion.

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)
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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.

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

 

Serial No. 5

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

 

Click the following link to get the model file:-  http://bit.ly/2m1eLaM

 

 Transcription of Video

1. Create a ‘New Assembly’ and save it with the name ‘Bevel Gear–Dynamic Simulation’.
2. Select Place component from the marking menu and place the Bevel 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 Top 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. Open the visibility of Y Axis of Assembly and Z Axis of Pinion from the Browser Bar and then apply a Mate Constraint between them.
11. Apply a Mate Constraint between Top Point of Assembly and Centre Point of Pinion from the Browser Bar.
12. 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.
13. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
14. Open the visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion.
15. 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.
16. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
17. Activate Insert Joint from the Marking menu.
18. Select ‘Rolling: Cone on Cone’ from the drop down menu of Insert Joint dialog box.
19. In the Insert Joint dialog box, select Pitch Diameter of Pinion in Component 1 and select Pitch Diameter of Gear in Component 2. 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 deg/s and click Ok.
24. Close the visibility of Pitch diameter of Bevel Gear and Pinion.
25. In Simulation Player fill the value 1000 in the Images field area.
26. Clear the screen by activating the Clean Screen command.
27. Click Run in the Simulation Player to display motion in Bevel Gear and Pinion.

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

Serial No. 46

Helical Gear (Internal)-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-Internal’.

 

 

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

 

 Transcription of Video

Display motion in Helical Gear (Internal) through Dynamic Simulation

1. Create a ‘New Assembly’ and save it with the name ‘Helical Gear (Internal)-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 only one Degree 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, and click OK.
11. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
12. Open the visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion.
13. Activate the Tangent Mate, change the Solution type to Inside, then select Pitch Diameter of Pinion and Pitch Diameter of Gear, and click OK.
14. Apply a Mate Constraint between the Z Axis of Pinion and YZ Plane of Assembly.
15. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Pinion.
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 Pinion 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 top face of Gear and then the top face of Pinion. In the Ratio input box, enter the value 23/57 and click Ok.
21. Once again, check the Degrees of Freedom of Helical 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 in Cylinder’ from the drop down menu of Insert Joint dialog box.
25. Select Rolling constraint option.
26. In the Insert Joint dialog box, select Pitch Diameter of Gear in ‘Outer Component option’ and select Pitch Diameter of Pinion in ‘Inner Component option’. Click Ok.
27. Select Revolution:2 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 deg/s and click Ok.
31. Close the visibility of Pitch diameter of Helical Gear and Pinion.
32. In Simulation Player, fill the value 1000 in the Images field area.
33. Clear the screen by activating the Clean Screen command.
34. Click Run in the Simulation Player to display motion in Helical Gear and Pinion.

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.

Rack and Pinion-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

  

Serial No. 79

Rack and Pinion-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

 

Click the following link to get the model file: - http://bit.ly/2muqD5w

 

 

 

Transcription of Video

Display motion in Rack and Pinion through Drive Constraint.

1. Create a ‘New Assembly’ and save it with the name ‘Rack and Pinion - Drive Constraint’.
2. Select Place component from the marking menu and place the Pinion in the Assembly.
3. Align the Pinion in correct position by using View Cube.
4. Select the Pinion in the design window, right click and uncheck its Grounded status in the Assembly.
5. Open the visibility of Z Axis of Assembly and Z Axis of Pinion from the Browser Bar.
6. Apply a Mate Constraint between Z Axis of Assembly and Z Axis of Pinion.
7. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Pinion.
8. Place the Rack in the Assembly and align it properly with Pinion by using Rotate Component Tool.
9. Apply a Tangent Mate between Pitch Circle of Pinion and Pitch Line of Rack.
10. Activate Angle Constraint, First select XZ Plane of Assembly, Second select XZ Plane of Rack and in the last Third select front face of Rack, click apply.
11. Open the visibility of YZ Plane of Pinion and Work Plane 7 of Rack; later apply a mate constraint between them.
12. Turn off the visibility of Work Plane to make the screen clear.
13. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
14. Right click the Mate:3 in the browser and select Supress from the context menu.
15. Open the visibility of YZ Plane of Pinion and YZ Plane of Assembly.
16. Activate the Angle Constraint, First select YZ Plane of Assembly, Second select YZ Plane of Pinion and in the last Third select front face of Rack, click apply.
17. Turn off the visibility of Work Plane to make the screen clear.
18. Activate the Motion constraint, in the Type area select Rotation-Translation, and afterwards select the Pitch Circle of Pinion then Pitch Line of Rack. Fill the 4.725 inch in the Distance Input box and click OK.
19. Select the Angle:2 Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
20. Right click the Drive Constraint and select Drive Constraint Tool from the context menu.
21. In the Drive Constraint dialog box, set the End value to 360 deg.
22. Expand the dialog box and set the value for Increment 0.25 deg.
23. Clear the screen by activating the Clean Screen command.
24. Click the Forward Button to display motion in Rack and Pinion.

Worm Gear-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 108

Worm Gear-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 ‘Worm Gear’.

 

Click the following link to get the model file: - http://bit.ly/2o3ZHKc

 

Transcription of Video

Display motion in Worm Gear through Drive Constraint.

1. Create a ‘New Assembly’ and save it with the name ‘Worm Gear - Drive Constraint’.
2. Hold the Ctrl key, and click the Worm Gear tool on the Power Transmission panel of the Design Tab.
3. The Worm Gears Component Generator dialog box will open with its default values. Click ok.
4. Click anywhere in the Design Window, to place the Worm and Worm Gear.
5. Align the model in correct position by using View Cube.
6. Make the Worm Gear Assembly flexible from the Browser Bar.
7. Open the Visibility of X Axis of Assembly and X Axis of Worm in the Browser; later apply a Mate Constraint between them.
8. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Worm.
9. Open the visibility of XY Plane of Assembly.
10. Place a Mate Constraint between XY Plane of Assembly and XY Plane of Worm Gear.
11. Place an Angle Constraint between XZ Plane of Worm and XY Plane of Assembly. In the solution field area, select Directed Angle option.
12. Turn off the visibility of Work Plane to make the screen clear.
13. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
14. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
15. Right click the Drive Constraint and select Drive Constraint Tool from the context menu.
16. In the Drive Constraint dialog box, set the End value to 360*10 deg.
17. Expand the dialog box and set the value for Increment 4 deg.
18. Clear the screen by activating the Clean Screen command.
19. Click the Forward Button to display motion in Worm and Worm Gear.

Bevel Gear-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 4

Bevel Gear-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will demonstrate how to create the 'Bevel Gear and Pinion' with the help of 'Bevel Gears Component Generator' command in the assembly. Application of the different type of mates in the assembly environment for creating the animation has been implemented through 'Drive Constraints' command.

 

Click the following link to get the model file:-  http://bit.ly/2nyXDK4

 

 Transcription of the Video

1. Create a ‘New Assembly’ and save it with the name ‘Bevel Gear - Drive Constraint’.
2. Hold the Ctrl key, and click the Bevel Gear tool on the Power Transmission panel of the Design tab.
3. The Bevel Gears Component Generator dialog box will open with its default values. Click ok.
4. Click anywhere in the Design Window, to place the Bevel Gear 2 and Bevel Gear 1.
5. Align the model in correct position by using View Cube.
6. Make the Bevel Gear Assembly flexible from the Browser Bar.
7. Apply a Mate Constraint between Z Axis of Bevel Gear 2 and the Y Axis of the Assembly.
8. Place a Mate Constraint between Centre Point of Assembly and Top Point of Bevel Gear 2.
9. Place another Mate Constraint between Z Axis of Assembly and Z Axis of Bevel Gear 1.
10. Open the visibility of XZ Plane of Bevel Gear 2.
11. Place an Angle Constraint between YZ Plane of Assembly and previously opened XZ Work Plane of Bevel Gear 2. In the solution field area, select Directed Angle option.
12. Turn off the visibility of Work Plane to make the screen clear.
13. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
14. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
15. Right click the Drive Constraint and select Drive Constraint Tool from the context menu.
16. In the Drive Constraint dialog box, set the End value to 360 deg.
17. Expand the dialog box and the set the value for Increment 0.25 deg.
18. Clear the screen by activating the Clean Screen command, Click the Forward Button to display motion in Bevel Gear 2 and Bevel Gear 1.

Helical Gear (Internal)-Drive Constrain-Autodesk Inventor 2012 (with caption and audio narration)

Serial No. 180

Helical Gear (Internal)-Drive Constrain-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 ‘Helical Gear (Internal)’

 

 

Click the following link to get the model file: - http://bit.ly/2nE3spH

 

 

 Transcription of Video

Display motion in Helical Gear (Internal) through Drive Constraint.

1. Create a ‘New Assembly’ and save it with the name ‘Helical Gear (Internal)-Drive Constraint ’.
2. Hold the Ctrl key, and click the Spur Gear tool on the Power Transmission panel of the Design Tab.
3. The Spur Gears Component Generator dialog box will open with its default values. Under the common area, fill 20 degree in the Helix Angle input box and select the check box next to ‘Internal’. Click ok.
4. Click anywhere in the Design Window, to place the Spur Gear 1 and Spur Gear 2.
5. Align the model in correct position by using View Cube.
6. Make the Spur Gear Assembly flexible from the Browser Bar.
7. Open the Visibility of Z Axis of Assembly and Z Axis of Spur Gear 1 in the Browser; later apply a Mate Constraint between them.
8. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Spur Gear 1.
9. Open the visibility of YZ Plane of Assembly and Z axis of Spur Gear 2; later apply a Mate Constraint between them.
10. Place an Angle Constraint between YZ Plane of Spur Gear 1 and YZ Plane of Assembly. In the solution field area, select Directed Angle option.
11. Turn off the visibility of Work Plane to make the screen clear.
12. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
13. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
14. Right click the Drive Constraint and select Drive Constraint Tool from the context menu.
15. In the Drive Constraint dialog box, set the End value to 360 deg.
16. Expand the dialog box and set the value for Increment 0.5 deg.
17. Clear the screen by activating the Clean Screen command.
18. Click the Forward Button to display motion in Spur Gear 1 and Spur Gear 2.

Tips:

In external Tooth systems, direction of rotation is in opposing directions.
Internal gears have a parallel direction of rotation and a small centre distance.

Helical Gear-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

  

Serial No. 47

Helical Gear-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)

 

 

Click the following link to get the model file: - http://bit.ly/2m6Gffr

 

 Transcription of Video

Display motion in Helical Gear through Drive Constraint.

1. Create a ‘New Assembly’ and save it with the name ‘Helical Gear - Drive Constraint’.
2. Hold the Ctrl key, and click the Spur Gear tool on the Power Transmission panel of the Design Tab.
3. The Spur Gears Component Generator dialog box will open with its default values. Fill 20 degree in Helix Angle field. Click ok.
4. Click anywhere in the Design Window, to place the Spur Gear 1 and Spur Gear 2.
5. Align the model in correct position by using View Cube.
6. Make the Spur Gear Assembly flexible from the Browser Bar.
7. Open the Visibility of Z Axis of Assembly and Z Axis of Spur Gear 1 in the Browser; later apply a Mate Constraint between them.
8. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Spur Gear 1.
9. Open the visibility of YZ Plane of Assembly and Z axis of Spur Gear 2; later apply a Mate Constraint between them.
10. Place an Angle Constraint between YZ Plane of Spur Gear 1 and YZ Plane of Assembly. In the solution field area, select Directed Angle option.
11. Turn off the visibility of Work Plane to make the screen clear.
12. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser.
13. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly.
14. Right click the Drive Constraint and select Drive Constraint Tool from the context menu.
15. In the Drive Constraint dialog box, set the End value to 360 deg.
16. Expand the dialog box and set the value for Increment 0.5 deg.
17. Clear the screen by activating the Clean Screen command.
18. Click the Forward Button to display motion in Spur Gear 1 and Spur Gear 2.

Application of Extrude Feature-Autodesk Inventor 2013 (with caption and audio narration)

 

Serial No.150

Application of Extrude Feature-Autodesk Inventor 2013 (with caption and audio narration)

In this Video, we have focused mainly on Extrude Feature and its application to make 'Part7' of previously created model 'LED Lamp'.

 

 

   

Click the following link to get the drawing sheet of the model: - http://bit.ly/2nL6ybg

 

 

Transcription of Video

Application of Extrude Feature

In this Video we have focused mainly on Extrude Feature and its application to make ‘Part7’ of previously created model ‘LED Lamp’.

1. At present you are watching a work piece in the design window. Its name is ‘Part7’ which is taken from our previously created model ‘LED Lamp’.
2. We want to develop this work piece like this.
3. In the following steps we will start adding some more features.
4. We will start our work by creating a new Work Plane that would be tangent to surface of this work piece.
5. Draw a new sketch on this Work Plane which is defined as sketch6 in the Browser.
6. Take the project of XY Plane with the help of ‘Project Geometry’ Tool.
7. Start a Rectangle Tool Command and fill the dimension.
8. Apply Coincident Constraint between the rectangle and vertical line.
9. Now the rectangle is centred over the vertical line.
10. Now take the project of this edge and convert it to construction mode.
11. Now apply Collinear Constraint between horizontal line of the rectangle and the construction line.
12. Now draw an arc over the top edge of this rectangle, next convert this line into the construction geometry.
13. Take another project of this edge.
14. Draw a line over this edge and centre align it with the vertical line.
15. Draw an arc again.
16. Apply the dimension as displayed.
17. Create a triangular shape drawing with given dimensions.
18. Now this sketch is complete.
19. Select Work Plane2, right click and turn off its visibility.
20. Extrude sketch6-a and select the ‘Cut’ option and click OK.
21. Fill the dimension 0.12475 inch to remove the unwanted material.
22. In the browser click the small plus icon beside the Extrusion5 and select Sketch6, right click and select share sketch, you will see that Sketch6 is visible. (By using ‘Share Sketch’ option we can reuse a previously drawn sketch feature).
23. Now activate the ‘Extrude’ feature once again and select Sketch6-b and cut this section.
24. Create a new sketch on this face.
25. Extrude the surface enclosed by inner circle and cut it by 1/8 inch.
26. Go to ‘Circular Pattern’ Tool, select Extrusion5 and Extrusion6 from the Browser Bar and define the axis of revolution by selecting the circular surface of this face and fill eight occurrences in the ‘Placement’ option and click OK.
27. Create a circular flat ring of width 1/32 inch and extrude this sketch to 1/4 inch.
28. Create one other circular strip of width 1/32 inch outside the previously created inner ring and extrude this sketch to 1/8 inch.
29. In the next step we go to ‘Shell’ Tool and select the desired face and fill thickness 1/32 inch and click OK.
30. Finally we found the desired shape of Part7.

Creating wires in Mesh of Table Fan-Autodesk Inventor 2013 (with caption and audio narration)

 

Serial No.149

Creating wires in Mesh of Table Fan-Autodesk Inventor 2013 (with caption and audio narration)
.......................................................................
This video will display how to create wires of the mesh of our previously created model 'Mesh of Table Fan'.

 

 

Click the following link to get the drawing sheet of the model: - http://bit.ly/2neUSNX

 

 Transcription of Video

Creating wires in Mesh of Table Fan

This video will display how to create wires of mesh of our previously created model ‘Mesh of Table Fan’.

1. At present there are three components Part1, Part2 and Part3 in the Assembly.
2. And we want to create 3 more new components Part4, Part5 and Part6 like this.
3. We will start our work with creating a new component in the Assembly.
4. At present the newly created component is not fully constrained in the Assembly, which can be confirmed by checking the ‘Degrees of Freedom’.
5. To fully constrain it in the Assembly, we will apply Mate Constraint between Center Point of Part4 and Center Point of Assembly.
6. Next, we will apply a Mate Constraint between Z Axis of Part4 and Z Axis of Assembly.
7. And finally a Mate Constraint between XZ Plane of Assembly and XZ Plane of Part4.
8. Now the Part is fully constrained, there are no Degrees of Freedom left.
9. In this Assembly, a ‘Component Pattern’ feature was applied to replicate the Part3.
10. We will ‘Suppress’ this feature and make visible only one instance of the Part3.
11. By double clicking the Part4, we will now enter in the Part Modelling environment.
12. Our first sketch will be drawn on the XZ Plane of Part4.
13. First we will project the edges of the other components available in the Assembly, using the ‘Project Cut Edges’ Command.
14. We will use these edges as a reference for creating new sketch. That is why we will apply a construction override on these projected edges. This will prevent them from being recognized as profiles by the 3D features.
15. This offset length is equal to the radius of wire of mesh.
16. Now we are applying constraints on our sketches to position it properly. This will also make our sketch Fully Constrained.
17. We will create a Work Point on this newly created sketch and replicate it 22 times with the use of ‘Rectangular Pattern’ Tool.
18. Select ‘Curve Length’ to place the Work Points along the path of the sketch.
19. Now start a new sketch on the XZ Plane of Part4.
20. Now project this Work Point on the sketch with the use of ‘Project Geometry’ Tool.
21. Draw a circle on this point.
22. Now we will develop our first wire of mesh with the help of ‘Revolve feature’.
23. Change the colour of Part4 to 'Steel'.
24. Repeat the same steps to generate other wires of mesh.
25. Clear the screen by activating the 'Clean Screen' Command.
26. The fully developed Assembly will look like this.

Creating hole on a curve surface-Autodesk Inventor 2013 (with caption and audio narration)

 

Serial No.148

Creating hole on a curve surface-Autodesk Inventor 2013 (with caption and audio narration)
..................................................................................
In this Video, we will show how to create holes on a Curved Surface using our Model 'Strainer'.

 

  

Click the following link to get the drawing sheet of the model: http://bit.ly/2o5IwIj

 

 

Transcription of Video

Creating hole on a curve surface

In this Video we will show how to create holes on a Curved Surface using our Model ‘Strainer’.

1. This is the model of ‘Strainer’ on which we want to create holes on it curved surface like this.
2. First of all, we will enter in the part modelling environment by double clicking the Part1.
3. We have already created Work Points on the curved surface of Strainer on the basis of a previously created sketch.
4. These are all the Work Points, which you can see in the Browser Bar as well as in the design window.
5. In the half section view, you can see it clearly that all the Work Points are landing on the curved face on the Strainer.
6. This is the sketch on the basis of which all the Work Points were created earlier.
7. A sketch of hole is required to create a hole on the Work Point.
8. So first of all we will create a Work Plane on the Work Point that would be tangent to the curved surface of the Strainer.
9. Take the project of Work Point and start the Circle Tool to create a circle of 0.03125 unit length.
10. Finish the sketch.
11. To create a hole on this sketch, we will use Extrude Command.
12. Click Extrude from the Create Panel of 3D Model Tab.
13. Click the circular profile.
14. In the direction field, select ‘Symmetric’ option.
15. Select ‘Cut’ option to remove the material from the curved surface of the Strainer and the hole is created.
16. Turn off the visibility of the Work Plane.
17. Now we will use the Circular Pattern Tool, that will replicate this extrude feature 80 times.
18. First select the feature then the rotation axis.
19. We will select the rotation axis as Y Axis from the Browser Bar.
20. In the Placement field type 80.
21. All the holes are now created.
22. In the same way, we will create another hole on this Work Point.
23. Same operations are being performed.
24. This time we will activate the Extrude Command by just clicking the sketch, here you can see.
25. The Extrude Command is visible there.
26. In the second row, the circumference of the model has decreased, so we have to select less number of holes (i.e., 78 occurrences) in this Circular Pattern.
27. In the same manner other holes can be created on the curved surface of the object easily, to get the desired result.
28. Here is the finished Assembly of the Strainer you can see all the holes are here.

Creating a component in an assembly-Autodesk Inventor 2013 (with caption and audio narration)

 

 

Serial No. 147

Creating a component in an assembly-Autodesk Inventor 2013 (with caption and audio narration)

This video will display how to create a component in the context of an Assembly. Creating a component in this way has many benefits. We can Project faces and edges of the Assembly in the new component.  The faces of other components can be copied and placed on surfaces and many more things can be done. So watch the video to understand.

 

 

Transcription of Video

Creating a component in an Assembly

This video will display how to create a component in the context of an Assembly. Creating a component in this way has many benefits. We can Project faces and edges of the Assembly in the new component. The faces of other components can be copied and placed as surfaces and many more things can be done. So watch the video to understand.

1. We have an Assembly named ‘Mesh (Front)’ consisting two components ‘Part1’ and ‘Part2’.
2. Now we want to create a new component named ‘Part3’ in this Assembly like this.
3. The Vertical distance between Part1 and Part2 is 1.625 inch.
4. We will start our work with creating a new component in this Assembly.
5. The degree of freedom command shows that the newly created Part3 is not fully constrained with the Assembly.
6. So we will apply a Mate Constraint between the Part3 and Assembly’s Z Axis.
7. Next a Mate Constraint will be applied between XZ Planes of Assembly and Part3.
8. In the following steps, we will create a loft feature in this component with the help of two sketches and a centre line rail.
9. By double clicking the Part3 we will enter in the Part Modelling Environment.
10. First of all we will get the edges of previously created components with the use of ‘Project Geometry Tool.’
11. These projected geometries are required only for reference. We are actually going to use these geometries in the developing the loft feature, that is why we will convert them in Construction Geometry.
12. By applying Coincident Constraint we will properly position our geometry.
13. Again unnecessary sketches will be converted into Construction Geometry.
14. So we have created the required sketch now.
15. Now we will create a New Work Plane parallel to YZ Plane of Part3 (7.625 inch away).
16. Now we will create the remaining sketch on the XZ Plane of the Part3 that will be used for Centre line loft.
17. From here we will change the colour of the Part to ‘Being Personal.’
18. In the next following steps we will develop the second loft feature in this Part.
19. At present we are copying the outer face of the Part2 with the ‘Copy Object’ Tool. This will place a new surface component in this part.
20. Now we will project this sketch on the previously created surface component with the help of ‘Project to 3D Sketch’ Tool.
21. At present this 3D sketch is intact. We cannot use its one edge as a rail in the loft feature. So we will create a new 3D sketch and project its one edge in it with the use of ‘Include Geometry’ Tool.
22. Repeat the same process to create the second Rail.
23. In this way, we found our two separate rails required for the loft.
24. Now we will create two 3D sketch profiles required for the loft.
25. So everything is set. Start the ‘Loft’ Tool.
26. Model edges can also be used as rails.
27. So in this way we created our second loft feature in the Part3.
28. We will now replicate this (Part3) 8 times at an angle of 45 degree by using ‘Pattern Component’ Tool, available at Component Panel of Assembly Tab.
29. If you want to watch the development of other components, used in the ‘Mesh of Table Fan’ Assembly, watch our previous video named ‘Mesh of Table Fan’ (Autodesk Inventor 2010).

Rotate and Place components in an Assembly-Autodesk Inventor 2013 (with caption and audio narration)

 

 

Serial No. 146

Rotate and Place components in an Assembly-Autodesk Inventor 2013 (with caption and audio narration)

In this Video we will describe about rotating and placing components in an Assembly.

Transcription of Video

Rotate and Place components in an Assembly

In this Video we will describe about rotating and placing components in an Assembly.

1. We have following components, which we want to place and constrain in an Assembly like this.
2. So create a New Assembly File and start placing the components.
3. The first component placed in an Assembly is always ‘Grounded’ and there is no need to constrain it.
4. Now we are going to place the ‘Part8’ in the Assembly.
5. To properly position the Part8 for Mate we will use ‘Rotate Component’ Command which is located in the Position Panel of Assemble Tab.
6. After selecting the Part8, click anywhere outside the reticle to start the rotation.
7. The component is positioned for the Mate now.
8. Start the ‘Constrain’ Tool.
9. Click this face and then this face.
10. Now click Apply.
11. The Rewind Tool is very useful to restore the most recent view or scroll through all of the save views.
12. In the same way, other four Parts can be placed, positioned and constrained to get the desired result…..
13. Now Assembly is fully constrained, there are no Degrees of Freedom that can be checked in this way…

Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 145

Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will describe 3D sketch and its application in the creation of loft feature.

 

Click the following link to get the drawing sheet of the model: http://bit.ly/2m51dLC

 

 

 Transcription of Video

Application of 3D sketch with loft feature

In this video we will describe about 3D sketch and its application in creation of loft feature.

1. This is our sketch which is named Sketch5 in the browser.
2. It is 2 inch up vertically from this point.
3. This sketch is placed on the Work Plane5.
4. Work Plane5 is 4.5 inch away from the Work Plane4.
5. Now we want to connect Sketch5 to the cup of the Spoon like this.
6. For this we will create two 3D sketches.
7. Start a 3D sketch from the Sketch panel of the Model Tab.
8. Create 3D line and close the sketch like this.
9. Once again create another 3D sketch in the same manner.
10. So the required two 3D sketches are in hand which we will use for developing the handle of Spoon.
11. Now pick up the loft tool from the Create panel of the Model Tab and develop the handle of Spoon like this.

Application of browser bar in Autodesk Inventor (with caption and audio narration)

 

 

Serial No. 144 

Application of browser bar in Autodesk Inventor (with caption and audio narration)

In this video, we will tell you about the Browser Bar of Autodesk Inventor Software and its use.
Autodesk Inventor is referred to as parametric solid modelling software. It maintains the history of how parts were constructed. The history will also show how they are related to one another in an Assembly. You can monitor this by observing the Browser Bar.

 

 

Transcription of Video

Application of Browser Bar in Autodesk Inventor

In this video we will tell you about the Browser Bar of Autodesk Inventor Software and its use.

Autodesk Inventor is referred to as parametric solid modelling software. It maintains the history of how parts were constructed. The history will also show how they are related to one another in an Assembly. You can monitor this by observing the Browser Bar.

Browser in Part Modelling Environment

How to observe history of parts.

1. Currently we are opening the model of Anvil.
2. This is the Browser Bar.
3. From here you can check, what the designing process of this CAD Model was.

Browser in Assembly Modelling Environment

How to observe relation of Parts in the Assembly

1. Currently we are opening the model of Shaving Razor.
2. In the case of Assembly you can understand the history of modelling as well as relation of parts to one another by exploring the Mate Constraints.

Application of Split Tool-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 143

Application of Split Tool-Autodesk Inventor 2012 (with caption and audio narration)
In this Video, we will describe 'Split' Tool and its application in cutting a segment from an intact face.

 

 

Click the following link to get the drawing sheet of the model: http://bit.ly/2m51dLC

 

 

Transcription of Video

Application of Split tool

In this Video we will describe about ‘Split’ Tool and its application in cutting a segment from an intact face.

1. At present this face of the Spoon is intact. We need a segment of this face according to our design like this.
2. To do so, first we will create a Work Plane on the top edge of the Spoon.
3. Now we will create a line of 0.25 inch on this Work Plane.
4. We will use the ends of this line to create new Work Planes later.
5. These newly created Work Planes will be used as Splitting Tool.
6. Now start the ‘Split’ Tool.
7. Select ‘Split Face’ option in the Split tool dialog box.
8. Select the Work Plane for the splitting tool.
9. Use the Select face button for faces.
10. Select the intact face of the Spoon and click Apply.
11. Repeat the same process for next split.
12. So this is the segment of face which was split.
13. We can change the colour of this face to yellow. So that it can be recognized easily.

Create Part from Sketch (Autodesk Inventor 2012)

Serial No. 178

Create Part from Sketch (Autodesk Inventor 2012)

 

Click the following link to get the model file: - http://bit.ly/2olrR3E