Cam and Follower-Dynamic Simulation-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 183 Cam and Follower-Dynamic Simulation-Autodesk Inventor 2013 (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 ‘Cam and Follower’. Click the following link to get the model file : – http://bit.ly/2maTL1C Transcription of Video Display of motion in ‘Cam and Follower’ through Dynamic Simulation Click the New icon under the Work tab in the Welcome Screen of Autodesk Inventor Professional 2013. Select Metric Template in the Create New File Dialogue Box. Create a Standard (mm).iam Assembly file. Save it with the name ‘Cam and Follower-Dynamic Simulation’. Select Place component from the marking menu and place the ‘Cam’ in the Assembly. Align the Cam in correct position by using View Cube. Set the current view as Home View by using the toggle next to View Cube. Select the Cam in the design window and remove its ‘Grounded’ position from the context menu. Click the Degrees of Freedom icon in the Visibility Panel of View Tab. At present there are six Degrees of Freedom in Cam and it can be moved in any direction in the Assembly. Apply an Axis Mate between the Z Axis of Assembly and Z Axis of Cam. Apply a Flush Mate between the XY Plane of Assembly and upper most front face (Red coloured) of Cam. Now this time only one ‘Degrees of Freedom’ persist and Cam can be moved only on its Z Axis. Place the ‘Follower’ in the Assembly. Re-orient the Follower against the Cam using Rotate Component Tool. Apply a Flush Mate between the upper most front face (Red coloured) of Cam and face of small pulley (Black coloured) of Follower. Apply a Mate Constraint between YZ Plane of Assembly and YZ Plane of Follower. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Click the view Tab and change the View of the model to ‘Shaded with Edges’ in the Visual Style drop down. Activate Insert Joint from the Marking menu. Select ‘Sliding: Cylinder Curve’ from the drop down menu of Insert Joint dialog box. Select the outer edge of Cam in ‘Curve’ selection option and select circular edge of small pulley of Follower in ‘Cylinder’ selection option. Click OK. Select Revolution:1 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*2 deg/s and click Ok. In Simulation Player fill the value 400 in the Images field area. Clear the screen by activating the Clean Screen command. Click Run in the Simulation Player to display motion in Cam and Follower.
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 Create a New ‘Standard (mm) .ipt’ Part file. At present Sketch1 is active by default. Use the Finish Sketch command to exit from sketching mode. Open the visibility of YZ Work Plane under the origin folder in the Browser Bar. Create a new Work Plane Parallel to YZ Plane at an offset distance of 323.623 mm. Create a new Sketch on XY Plane. Draw a Circle of 97.021 mm diameter, coincident with the auto projected part origin. Create another Circle of 72.766 mm diameter. The distance between these two circles is 323.623 mm. Take the project of X Axis and convert it to construction geometry. The centre of small circle is 12.128 mm below the projected X Axis line. Draw a line connecting top of two circles as displayed. Take the project of YZ Plane and convert it to construction geometry. Draw another line between two circles. Erase the unwanted sketches by using the Trim tool. Apply dimensions to fully constraint the sketch as displayed. Take the project of Work Plane1 from the browser bar, with use of Project Geometry tool. Convert this line into construction geometry. Apply a dimension between these two projected lines. This dimension is driven dimension. Now the sketch is complete, exit the sketch environment. Create a Work Point at the intersection of YZ Plane and bottom line of the sketch. Activate the Parameters tool from the Parameters Panel of the Manage tab. Create a User defined Parameter named ‘start’ by clicking ‘Add Numeric’ button in the Parameters dialog box. Click the ‘Equation’ column and then select the driven dimension in the design window. Click Done. Save the Part file with the name ‘Locus of Tooth’. Start the Rectangular Pattern Tool and select Work Point1 in the Browser Bar as feature. Click the ‘Direction 1’ button and select the sketch in the design window. In the Column spacing input box, click arrow button to expand choices. Select List Parameters then select the ‘start’. Click more button to expand the dialogue box. Select Adjust in the ‘Compute’ option. Click the Start button in the ‘Direction 1’ field and select the Work Point1 in the Browser Bar. Click OK. Open the visibility of Sketch2 from the Browser Bar. Select Work Plane1 in the Browser Bar and make it ‘Adaptive’ from the context menu. Activate Rectangular Pattern Tool once again. Select Work Point2 in the Browser Bar as feature. Click the ‘Direction 1’ button and select the sketch in the design window. In the Column Count input box, enter the value 72. Click this drop down to specify pattern length. Select ‘Curve Length’ option. Click the more button to expand the dialogue box. Select Adjust in the ‘Compute’ option. Click the Start button in the ‘Direction 1’ field and select the Work Point2. Select Direction1 in the ‘Orientation’ option. Click OK. Save the file and close it. Create a ‘‘Standard (mm) .iam’ assembly’ and save it with the name ‘Synchronous Belt -Inventor Studio’. Select ‘Place component’ tool from the marking menu and place the ‘Locus of Tooth’ Part in the Assembly. Select the ‘Locus of Tooth’ Sketch from the Browser Bar, right click and deselect Grounded from the context menu. Select the ‘Locus of Tooth’ Sketch again and make it ‘Adaptive’ from the context menu. Align the model in appropriate position using the View Cube. Apply a Flush Mate between YZ Plane of Assembly and YZ Plane of Locus of Tooth. Apply a Flush Mate between XZ Plane of Assembly and XZ Plane of Locus of Tooth. Apply a Flush Mate between XY Plane of Assembly and XY Plane of Locus of Tooth. Apply a Mate Constraint between YZ Plane of Assembly and Work Plane1 of Locus of Tooth. Inter the value 323.623 mm in the Offset input box. Click OK. Select ‘Place component’ tool from the marking menu and place the ‘Tooth’ part in the Assembly. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Apply a Mate Constraint between Work Point2 of ‘Tooth’ and Work Point2 of ‘Locus of Tooth’. Change the view of design window by using View Cube. Apply a Flush Mate between XY Plane of Assembly and XY Plane of ‘Tooth’. Apply an Angle Constraint between XZ Plane of Assembly and XZ Plane of ‘Tooth’. Select Directed Angle option in the solution field. Close the visibility of Work Planes, visible in the design window. Create a Work Axis in the Assembly on this point, parallel to Z Axis of the Assembly. Place the ‘Belt-Base’ in the Assembly. Apply a Mate Constraint between Z Axis of Assembly and Z Axis of Belt-Base. Apply an Axis Mate between Belt-Base and Work Axis1 of Assembly. Apply a Mate Constraint between XY Plane of Assembly and XY Plane of Belt-Base. Start the Pattern Component Tool from the Component Panel of Assemble tab. Select the ‘Tooth’ as component, then select Rectangular Pattern2 of Locus of Tooth in the Browser Bar as Associative Feature Pattern. Click OK. Now all the ‘Teeth’ are fitted on the Locus of Teeth. Select ‘Place component’ from the marking menu and place the ‘Small Pulley’ in the Assembly. Apply a Mate Constraint between Z Axis of ‘Small Pulley’ and Work Axis1 of the Assembly. Apply a Mate Constraint between XY Plane of ‘Small Pulley’ and XY Plane of the Assembly. Select ‘Place component’ from the marking menu and place the ‘Large Pulley’ in the Assembly. Apply a Mate Constraint between Z Axis of ‘Large Pulley’ and Z Axis of the Assembly. Apply a Mate Constraint between XY Plane of Assembly
Ceiling Hook-Autodesk Inventor 2013 (with caption and audio narration)
Serial No. 16 Ceiling Hook-Autodesk Inventor 2013 (with caption and audio narration) Click the following link to get the model file: – http://bit.ly/2mcyc0m Transcription of Video Ceiling Hook: — Modelling and apply motion in it through Drive Constraint Create a New ‘Standard (in).ipt’ Part file. Create a new sketch on XY Plane of Part. Draw a Circle of 0.43800 inch diameter, coincident with Auto projected part origin. Draw a Line of length 0.25 inch parallel to Y axis. The midpoint of this line should lie on the X axis. Apply a Coincident Constraint between the end point of the line and the periphery of the circle. Create a new Line by taking the offset of this chord. Give the dimension of 0.15625 inch on this line. This line should be 1.5 inch away from the chord and its midpoint should lie on X axis. Start Line tool and join both the ends of this line with the end points of chord of circle. Convert all the sketches into construction geometry. Start the Centre Point Arc tool. Select the Auto projected part origin first then the end points of chord of the circle. Finish the sketch by clicking the Finish Sketch Icon. Create a new sketch on XZ plane. Take the project of last drawn arc and convert it to construction geometry. Create a circle of .094 inch diameter on the end point of this projected line. Finish the sketch. Activate Sweep Tool from the Create Panel of Model Tab. It will automatically select the small circle created on the Sketch2 as Profile and arc drawn on Sketch1 as path. Click OK. Change the Model colour to Flaked Reflective-Beige. Save the Part file with the name ‘Hook’. Open the visibility of Sketch1 in Browser Bar. Create a new Work Plane on this point parallel to YZ Plane of the Part. Draw a sketch on this work plan. Take the project of end point of the vertical line. Draw a Circle of 0.0625 inch diameter. Finish the sketch. Start Loft Tool, select small circle and circular edge of the part. Click OK. Close the visibility of Sketch1 and Work Plane1. Start Mirror tool from the Pattern panel of Model Tab. Select Loft1 from the Browser Bar as feature. Select XZ Plane from the Browser Bar as Mirror Plane. Click OK. Save the file and close it. Create a New ‘Standard (in).ipt’ Part file. Create a new sketch on XY Plane of Part. Draw a Circle of 1 inch diameter, coincident with Auto projected part origin. Finish the sketch by clicking the Finish Sketch Icon. Create a new sketch on XZ plane. Take the Project of big circle and convert it to construction geometry. Create a circle of 0.094 inch diameter on the end point of this projected line. Finish the sketch. Start Sweep Tool, select small circle as profile and select big circle as path. Click OK. Change the Model colour to Flaked Reflective-Beige. Save the file with the name ‘Circular Ring’ and close it. Create a New ‘Standard (in).iam’ Assembly and Save it with the name ‘Ceiling Hook’. Select Place Component from the marking menu and place the ‘Hook’ in the Assembly. Place ‘Circular Ring’ in the Assembly. Align the Circular Ring according to Hook by using Rotate Component Tool. Apply a Tangent Mate between Circular Ring and Hook. Apply a Mate Constraint between XY Plane of Assembly and YZ Plane of Circular Ring. Edit the Circular Ring in the Assembly by double clicking it. Activate Work Axis Command. First select the Centre Point of Hook, then the Z Axis of Hook from the Browser Bar. In this way a new Work Axis which is Adaptive to Z Axis of Hook is created. Return to Assembly by clicking Return Icon. Suppress the Tangent Mate from the Browser Bar, which was applied earlier. Now the Circular Ring is ready to move along the Hook. Create an Axis in the Assembly on the basis of two points on the periphery of Hook as displayed. Go to Work Features panel and click the drop down of Work Plane command. Select ‘Angle to Plane around Edge’ command. First select XY Plane of Assembly, then select Work Axis1 of Assembly. Click OK. Activate an Angle Constraint, first select Work Plane1 of the Assembly, then select XY Plane of Circular Ring and at last select XY Plane of Assembly. Click OK. Open the visibility of XZ Plane of Assembly. Measure the Angle between XZ Plane of Assembly and Work Plane1 of Assembly. The magnitude of this angle is 145.2 degree. Click the Selection drop drown menu and choose ‘Select Sketch Features’ command in the Quick Access Toolbar. Close the visibility of unnecessary work planes and work axis. Set the browser from Assembly View to Modeling View by using the Toggle at the top of the Browser Bar. Select the Angle:2 constraint under the Constraints folder in the Browser Bar 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 (145.2*2) degree. Click the more button to expand the dialog box, enter the value 0.5 degree in the ‘Increment’ field. Clear the screen by activating the Clean Screen command. Click the Forward Button to display motion in ‘Ceiling Hook’. Click Reverse Button to return at previous position.
