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 Create a ‘New Assembly’ and save it with the name ‘Bevel Gear–Dynamic Simulation’. Select Place component from the marking menu and place the Bevel Gear in the Assembly. Align the Gear in correct position by using View Cube. Select the Gear in the Design window, right click and deselect Grounded from the context menu. At present there are six Degrees of Freedom in Gear and it can be moved in any direction in the Assembly. 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. Apply another Mate Constraint between Centre point of the Assembly and Top point of the Gear. Now this time only one Degrees of Freedom is left and Gear can be moved only on its Z Axis. Select Place component from the marking menu and place the Pinion in the Assembly. 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. Apply a Mate Constraint between Top Point of Assembly and Centre Point of Pinion from the Browser Bar. 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. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Open the visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion. 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. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Activate Insert Joint from the Marking menu. Select ‘Rolling: Cone on Cone’ from the drop down menu of Insert Joint dialog box. 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. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option. Click the arrow to expand the input choices, and click Constant Value. Enter the value 360 deg/s and click Ok. Close the visibility of Pitch diameter of Bevel Gear and Pinion. In Simulation Player fill the value 1000 in the Images field area. Clear the screen by activating the Clean Screen command. 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 Create a ‘New Assembly’ and save it with the name ‘Helical Gear (Internal)-Dynamic Simulation’. Select Place component from the marking menu and place the Helical Gear in the Assembly. Align the Gear in correct position by using View Cube. Select the Gear in the Design window, right click and deselect Grounded from the context menu. At present there are six Degrees of Freedom in Gear and it can be moved in any direction in the Assembly. 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. Apply another Mate Constraint between Centre Point of the Assembly and Centre Point of the Gear. Now only one Degree of Freedom is left and Gear can be moved only on its Z Axis. Select Place component from the marking menu and place the Pinion in the Assembly. 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. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Open the visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion. Activate the Tangent Mate, change the Solution type to Inside, then select Pitch Diameter of Pinion and Pitch Diameter of Gear, and click OK. Apply a Mate Constraint between the Z Axis of Pinion and YZ Plane of Assembly. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Pinion. 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. Select Pitch Diameter of Pinion to create the Work Axis. In the Quick Access toolbar, click the selection tool dropdown list and choose Select Sketch Features. Convert this Work Axis to ‘Grounded’. 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. 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. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Select Insert Joint in the Marking menu. Select ‘Rolling: Cylinder in Cylinder’ from the drop down menu of Insert Joint dialog box. Select Rolling constraint option. 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. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option. Click the arrow to expand the input choices, and click Constant Value. Enter the value 360 deg/s and click Ok. Close the visibility of Pitch diameter of Helical Gear and Pinion. In Simulation Player, fill the value 1000 in the Images field area. Clear the screen by activating the Clean Screen command. 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 Create a ‘New Assembly’ and save it with the name ‘Helical Gear–Dynamic Simulation’. Select Place component from the marking menu and place the Helical Gear in the Assembly. Align the Gear in correct position by using View Cube. Select the Gear in the Design window, right click and deselect Grounded from the context menu. At present there are six Degrees of Freedom in Gear and it can be moved in any direction in the Assembly. 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. Apply another Mate Constraint between Centre point of the Assembly and Centre point of the Gear. Now this time only one Degrees of Freedom is left and Gear can be moved only on its Z Axis. Select Place component from the marking menu and place the Pinion in the Assembly. 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. Apply a Mate Constraint between YZ Plane of Gear and YZ Plane of Pinion. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Open visibility of Pitch Diameter of Gear and Pitch Diameter of Pinion and then apply a Tangent Mate between them. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Pinion. 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. Select Pitch Diameter of Pinion to create the Work Axis. In the Quick Access toolbar, click the selection tool dropdown list and choose Select Sketch Features. Convert this Work Axis to ‘Grounded’. 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. Suppress the Mate:3 Constraint in the Browser. 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. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Select Insert Joint in the Marking menu. Select ‘Rolling: Cylinder on Cylinder’ from the drop down menu of Insert Joint dialog box. Select Rolling constraint option. First select the Pitch Diameter of Pinion and then the Pitch Diameter of Gear. Click Ok. Select Revolution:3 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option. Click the arrow to expand the input choices, and click Constant Value. Enter the value 360.000 deg/s, and click Ok. In the Images field, enter the value 1000. Close the visibility of Pitch diameter of Helical Gear and Pinion. Mesh the teeth of Gear and Pinion manually in front of each other, after Suppressing the Motion Constraint. Once again Un-suppress the Motion Constraint. Clear the screen by activating the Clean Screen command. 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. Create a ‘New Assembly’ and save it with the name ‘Rack and Pinion – Drive Constraint’. Select Place component from the marking menu and place the Pinion in the Assembly. Align the Pinion in correct position by using View Cube. Select the Pinion in the design window, right click and uncheck its Grounded status in the Assembly. Open the visibility of Z Axis of Assembly and Z Axis of Pinion from the Browser Bar. Apply a Mate Constraint between Z Axis of Assembly and Z Axis of Pinion. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Pinion. Place the Rack in the Assembly and align it properly with Pinion by using Rotate Component Tool. Apply a Tangent Mate between Pitch Circle of Pinion and Pitch Line of Rack. 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. Open the visibility of YZ Plane of Pinion and Work Plane 7 of Rack; later apply a mate constraint between them. Turn off the visibility of Work Plane to make the screen clear. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Right click the Mate:3 in the browser and select Supress from the context menu. Open the visibility of YZ Plane of Pinion and YZ Plane of Assembly. 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. Turn off the visibility of Work Plane to make the screen clear. 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. Select the Angle:2 Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly. Right click the Drive Constraint and select Drive Constraint Tool from the context menu. In the Drive Constraint dialog box, set the End value to 360 deg. Expand the dialog box and set the value for Increment 0.25 deg. Clear the screen by activating the Clean Screen command. 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. Create a ‘New Assembly’ and save it with the name ‘Worm Gear – Drive Constraint’. Hold the Ctrl key, and click the Worm Gear tool on the Power Transmission panel of the Design Tab. The Worm Gears Component Generator dialog box will open with its default values. Click ok. Click anywhere in the Design Window, to place the Worm and Worm Gear. Align the model in correct position by using View Cube. Make the Worm Gear Assembly flexible from the Browser Bar. Open the Visibility of X Axis of Assembly and X Axis of Worm in the Browser; later apply a Mate Constraint between them. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Worm. Open the visibility of XY Plane of Assembly. Place a Mate Constraint between XY Plane of Assembly and XY Plane of Worm Gear. Place an Angle Constraint between XZ Plane of Worm and XY Plane of Assembly. In the solution field area, select Directed Angle option. Turn off the visibility of Work Plane to make the screen clear. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly. Right click the Drive Constraint and select Drive Constraint Tool from the context menu. In the Drive Constraint dialog box, set the End value to 360*10 deg. Expand the dialog box and set the value for Increment 4 deg. Clear the screen by activating the Clean Screen command. 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 Create a ‘New Assembly’ and save it with the name ‘Bevel Gear – Drive Constraint’. Hold the Ctrl key, and click the Bevel Gear tool on the Power Transmission panel of the Design tab. The Bevel Gears Component Generator dialog box will open with its default values. Click ok. Click anywhere in the Design Window, to place the Bevel Gear 2 and Bevel Gear 1. Align the model in correct position by using View Cube. Make the Bevel Gear Assembly flexible from the Browser Bar. Apply a Mate Constraint between Z Axis of Bevel Gear 2 and the Y Axis of the Assembly. Place a Mate Constraint between Centre Point of Assembly and Top Point of Bevel Gear 2. Place another Mate Constraint between Z Axis of Assembly and Z Axis of Bevel Gear 1. Open the visibility of XZ Plane of Bevel Gear 2. 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. Turn off the visibility of Work Plane to make the screen clear. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly. Right click the Drive Constraint and select Drive Constraint Tool from the context menu. In the Drive Constraint dialog box, set the End value to 360 deg. Expand the dialog box and the set the value for Increment 0.25 deg. 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. Create a ‘New Assembly’ and save it with the name ‘Helical Gear (Internal)-Drive Constraint ’. Hold the Ctrl key, and click the Spur Gear tool on the Power Transmission panel of the Design Tab. 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. Click anywhere in the Design Window, to place the Spur Gear 1 and Spur Gear 2. Align the model in correct position by using View Cube. Make the Spur Gear Assembly flexible from the Browser Bar. 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. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Spur Gear 1. Open the visibility of YZ Plane of Assembly and Z axis of Spur Gear 2; later apply a Mate Constraint between them. 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. Turn off the visibility of Work Plane to make the screen clear. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly. Right click the Drive Constraint and select Drive Constraint Tool from the context menu. In the Drive Constraint dialog box, set the End value to 360 deg. Expand the dialog box and set the value for Increment 0.5 deg. Clear the screen by activating the Clean Screen command. 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. Create a ‘New Assembly’ and save it with the name ‘Helical Gear – Drive Constraint’. Hold the Ctrl key, and click the Spur Gear tool on the Power Transmission panel of the Design Tab. The Spur Gears Component Generator dialog box will open with its default values. Fill 20 degree in Helix Angle field. Click ok. Click anywhere in the Design Window, to place the Spur Gear 1 and Spur Gear 2. Align the model in correct position by using View Cube. Make the Spur Gear Assembly flexible from the Browser Bar. 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. Place a Mate Constraint between Centre Point of Assembly and Centre Point of Spur Gear 1. Open the visibility of YZ Plane of Assembly and Z axis of Spur Gear 2; later apply a Mate Constraint between them. 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. Turn off the visibility of Work Plane to make the screen clear. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select the Angle Constraint in the Browser and change its name as ‘Drive’ by clicking twice slowly. Right click the Drive Constraint and select Drive Constraint Tool from the context menu. In the Drive Constraint dialog box, set the End value to 360 deg. Expand the dialog box and set the value for Increment 0.5 deg. Clear the screen by activating the Clean Screen command. 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’. 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’. We want to develop this work piece like this. In the following steps we will start adding some more features. We will start our work by creating a new Work Plane that would be tangent to surface of this work piece. Draw a new sketch on this Work Plane which is defined as sketch6 in the Browser. Take the project of XY Plane with the help of ‘Project Geometry’ Tool. Start a Rectangle Tool Command and fill the dimension. Apply Coincident Constraint between the rectangle and vertical line. Now the rectangle is centred over the vertical line. Now take the project of this edge and convert it to construction mode. Now apply Collinear Constraint between horizontal line of the rectangle and the construction line. Now draw an arc over the top edge of this rectangle, next convert this line into the construction geometry. Take another project of this edge. Draw a line over this edge and centre align it with the vertical line. Draw an arc again. Apply the dimension as displayed. Create a triangular shape drawing with given dimensions. Now this sketch is complete. Select Work Plane2, right click and turn off its visibility. Extrude sketch6-a and select the ‘Cut’ option and click OK. Fill the dimension 0.12475 inch to remove the unwanted material. 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). Now activate the ‘Extrude’ feature once again and select Sketch6-b and cut this section. Create a new sketch on this face. Extrude the surface enclosed by inner circle and cut it by 1/8 inch. 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. Create a circular flat ring of width 1/32 inch and extrude this sketch to 1/4 inch. Create one other circular strip of width 1/32 inch outside the previously created inner ring and extrude this sketch to 1/8 inch. In the next step we go to ‘Shell’ Tool and select the desired face and fill thickness 1/32 inch and click OK. 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’. At present there are three components Part1, Part2 and Part3 in the Assembly. And we want to create 3 more new components Part4, Part5 and Part6 like this. We will start our work with creating a new component in the Assembly. At present the newly created component is not fully constrained in the Assembly, which can be confirmed by checking the ‘Degrees of Freedom’. To fully constrain it in the Assembly, we will apply Mate Constraint between Center Point of Part4 and Center Point of Assembly. Next, we will apply a Mate Constraint between Z Axis of Part4 and Z Axis of Assembly. And finally a Mate Constraint between XZ Plane of Assembly and XZ Plane of Part4. Now the Part is fully constrained, there are no Degrees of Freedom left. In this Assembly, a ‘Component Pattern’ feature was applied to replicate the Part3. We will ‘Suppress’ this feature and make visible only one instance of the Part3. By double clicking the Part4, we will now enter in the Part Modelling environment. Our first sketch will be drawn on the XZ Plane of Part4. First we will project the edges of the other components available in the Assembly, using the ‘Project Cut Edges’ Command. 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. This offset length is equal to the radius of wire of mesh. Now we are applying constraints on our sketches to position it properly. This will also make our sketch Fully Constrained. We will create a Work Point on this newly created sketch and replicate it 22 times with the use of ‘Rectangular Pattern’ Tool. Select ‘Curve Length’ to place the Work Points along the path of the sketch. Now start a new sketch on the XZ Plane of Part4. Now project this Work Point on the sketch with the use of ‘Project Geometry’ Tool. Draw a circle on this point. Now we will develop our first wire of mesh with the help of ‘Revolve feature’. Change the colour of Part4 to ‘Steel’. Repeat the same steps to generate other wires of mesh. Clear the screen by activating the ‘Clean Screen’ Command. The fully developed Assembly will look like this.
