Pipe Wrench-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 182 Pipe Wrench-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Pipe Wrench’. Click the following link to get the model file: – http://bit.ly/2mT1v8y Transcription of Video Display of Motion in ‘Pipe Wrench’ through Dynamic Simulation. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Pipe Wrench-Dynamic Simulation’. Select Place component from the marking menu and place the ‘Base Frame’ in the Assembly. Re-orient the model in the design window by using View Cube. Set the current view as Home View by using the toggle next to View Cube. Place the ‘Supporting Bracket’ in the Assembly. Apply an Axis Mate between hole on the Base Frame and hole on the Supporting Bracket. Apply a Flush Mate Between XY Plane of Base Frame and XY Plane of Supporting Bracket. Activate Angle Constraint Command first select side face of Base Frame; then select side face of Supporting Bracket and at the last select top face of Supporting Bracket. Enter the value -4.76 degree in the Angle Input Box and click OK. Place the ‘Rivet-1’ in the Assembly. Fix the Rivet-1 in the hole of Supporting Bracket by the use of Insert Mate as displayed. Place the ‘Supporting Strip-1’ in the Assembly. Place the Supporting Strip -1 on the hole of Base Frame with the help of Insert Mate. Apply an Angle Constraint between top face of Supporting Strip -1 and top face of Base Frame. In the Solution Type, select Directed Angle. Place the ‘Rivet-2’ in the Assembly. Fix the Rivet-2 on the hole of Supporting Strip-1 with the help of Insert Mate. Place the ‘Supporting Strip-2’ in the Assembly. Place the Supporting Strip -2 on the hole of Base Frame with the help of Insert Mate. Apply an Angle Constraint between top face of Supporting Strip -2 and top face of Base Frame. In the Solution Type, select Directed Angle. Drag the Rivet-2 from the Browser Bar in the Assembly. This will place a copy of Rivet-2 in the Assembly. Fix the Rivet-2 on the hole of Supporting Strip-2 with the help of Insert Mate. Place the ‘Sliding Frame’ in the Assembly. Apply a Flush Mate between XY Plane of Base Frame and XY Plane of Sliding Frame. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Apply a Mate Constraint between X Axis of Sliding Frame and Work Plane 7 of Supporting Bracket. Place the ‘Wheel’ in the Assembly. Apply a Mate Constraint between X Axis of Sliding Frame and Axis of Wheel. Apply a Mate Constraint between Work Plane 5 of Supporting Bracket and Work Plane 1 of Wheel. Apply a Mate Constraint between Jaw of Base Frame and Jaw of Sliding Frame in the Assembly. Select the previous applied ‘Mate: 5’ under the Constraints folder in the Browser Bar, Right click and choose ‘Supress’ from the context menu. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Select Insert Joint in the Marking menu. Select ‘Screw’ from the drop down menu of Insert Joint dialog box. In the Insert Joint dialog box, select Circular edge of Sliding Frame in ‘Component 1’ selection option and select Circular edge of Wheel in ‘Component 2’ selection option. Enter the value 0.205 in the ‘Pitch’ input box. 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 (-360/0.205) deg/s and click OK. 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 Pipe Wrench.
Pipe Wrench-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 75 Pipe Wrench-Drive Constraint-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation of the ‘Pipe Wrench’. Click the following link to get the model file: – http://bit.ly/2njQE7E Transcription of Video Display of Motion in ‘Pipe Wrench’ through Drive Constraint. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Pipe Wrench-Drive Constraint’. Select Place component from the marking menu and place the ‘Base Frame’ in the Assembly. Re-orient the model in the design window by using View Cube. Set the current view as Home View by using the toggle next to View Cube. Place the ‘Supporting Bracket’ in the Assembly. Apply an Axis Mate between hole on the Base Frame and hole on the Supporting Bracket. Apply a Flush Mate Between XY Plane of Base Frame and XY Plane of Supporting Bracket. Activate Angle Constraint Command first select side face of Base Frame; then select side face of Supporting Bracket and at the last select top face of Supporting Bracket. Enter the value -4.76 degree in the Angle Input Box and click OK. Place the ‘Rivet-1’ in the Assembly. Fix the Rivet-1 in the hole of Supporting Bracket by the use of Insert Mate as displayed. Place the ‘Supporting Strip-1’ in the Assembly. Place the Supporting Strip -1 on the hole of Base Frame with the help of Insert Mate. Apply an Angle Constraint between top face of Supporting Strip -1 and top face of Base Frame. In the Solution Type, select Directed Angle. Place the ‘Rivet-2’ in the Assembly. Fix the Rivet-2 on the hole of Supporting Strip-1 with the help of Insert Mate. Place the ‘Supporting Strip-2’ in the Assembly. Place the Supporting Strip -2 on the hole of Base Frame with the help of Insert Mate. Apply an Angle Constraint between top face of Supporting Strip -2 and top face of Base Frame. In the Solution Type, select Directed Angle. Drag the Rivet-2 from the Browser Bar in the Assembly. This will place a copy of Rivet-2 in the Assembly. Fix the Rivet-2 on the hole of Supporting Strip-2 with the help of Insert Mate. Place the ‘Sliding Frame’ in the Assembly. Apply a Flush Mate between XY Plane of Base Frame and XY Plane of Sliding Frame. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Apply a Mate Constraint between X Axis of Sliding Frame and Work Plane 7 of Supporting Bracket. Place the ‘Wheel’ in the Assembly. Apply a Mate Constraint between X Axis of Sliding Frame and Axis of Wheel. Apply a Mate Constraint between Work Plane 5 of Supporting Bracket and Work Plane 1 of Wheel. Activate the Motion constraint, in the Type area select Rotation-Translation, and afterwards select the front face of Wheel then Vertical edge of Sliding Frame. Enter the value 0.205 inch in the Distance Input box and click OK. Activate the Angle Constraint, First select YZ Plane of Wheel, Second select XY Plane of Assembly and at last select top face of Supporting Bracket, and click OK. Apply a Mate Constraint between Jaw of Base Frame and Jaw of Sliding Frame in the Assembly. Select the previous applied ‘Mate: 5’ under the Constraints folder in the Browser Bar, Right click and choose ‘Supress’ from the context menu. Select the Angle:4 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 (360/0.205). Clear the screen by activating the Clean Screen command. Click the Forward Button to display motion in ‘Pipe Wrench’. To close the Jaw, click Reverse Button.
Hinge-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 49 Hinge-Autodesk Inventor 2012 (with caption and audio narration) Click the following link to get the model file: – http://bit.ly/2lHZ1cO Transcription of Video Hinge Modelling and apply motion in it through Drive-Constraint. Create a New ‘Standard (in).ipt’ Part file. Sketch1 is active by default. Draw a Rectangle 1.25 in. x 0.0625 in., coincident with Auto project part origin. Draw a Circle of 0.375 in. diameter. Apply a Tangent Constraint between circle and base line of the rectangle. Apply a Vertical Constraint between centre point of Circle and Auto project part origin. Draw another Circle of 0.25 in. diameter, Concentric with the previous one. Finish the Sketch. Start the Extrude command, select rectangle and the profile formed between the two circles. Enter the distance value 5 in. and select Symmetric option in the direction field. Click OK. Change the existing colour of the part into Popcorn. Save the file with the name Part 1. Create a new work plane 1 in. away from the front face of part. Start a new sketch on this Work Plane. Take the project of this edge of the part with Project Geometry Tool. Right click in the design window and select Slice Graphic from the context menu. By doing so hidden sketches behind the part will be seen clearly. Draw two lines to close the profile. Finish the Sketch. Start the Extrude command. It will automatic select the last drawn sketch profile, choose Cut option to remove the material from the part. Enter the distance value 1 in. Click ok. Start the Rectangular Pattern tool. Select Extrusion2 in the design window as feature. Click the ‘Direction 1’ button, and then select the outer edge of the Part1. Enter the value 2 in the column count input box. Enter the value 2 in. in the column spacing input box. Click OK. Take the project of edges of the model. Draw a rectangle coincident with the end point of the projected lines. Start the Offset tool, select the rectangle and drag the profile inside. A new Rectangle will be created. Place the dimension .25 in. as offset distance between the two rectangles. Start the Rectangular Pattern tool. Select bottom line of the rectangle. Click the ‘Direction 1’ button, and then select the vertical line of the rectangle. Click Flip button to change the direction of pattern. Enter the value 4 in the column count input box. Click the arrow button to expand the input choices in the column spacing input box. Choose ‘Measure’ option then select the vertical line of rectangle. Click more button to expand the dialogue box. Select ‘Fitted’ option and click OK. Convert all sketches into construction geometry. Hold the Ctrl Key and select the end points of these lines and convert them to centre point. Start the Hole Tool. The Points which we converted into centre point will be automatically selected. Set the diameter of the hole to 0.125 in. In the termination drop down menu select Through All option and Click OK. Start the Chamfer Tool. Select the top edges of all the holes. Enter the value 1/32 in. in the Distance field. Click OK. Save the file. Save As the same file with the name Part 2 also. This file will be used later in creation of Hinge Assembly. Close the file. Create a New Standard (in).iam Assembly file. Place the ‘Part 1’ file in the Assembly with aid of Place Component Tool. Save the Assembly with name ‘Hinge’. Place the ‘Part 2’ in the Assembly. Align ‘Part 2’ in correct position by using Rotate Component Tool. Some modifications are needed here in ‘Part 2’, so as to match it with Part 1. Select the Part 2 and double click it, to edit in the part modelling environment. Edit the Extrusion2 feature in the Browser Bar by double clicking it. In the Extrude2 dialogue box, change the direction of extrusion. In the same way, edit the Rectangular Pattern1. In the Column count input box, enter the value 3 and click OK. Click the Return icon, to return back in the Assembly modelling environment. Apply a mate constraint between the Axis of Part 1 and Part 2. Apply a Flush mate between the Front face of Part 1 and Part2. Right Click in the design window and select Create Component Tool from the marking menu. Give name of the part as ‘Centre Pin’. Click Ok. Select XY plane of Assembly, as a base plane for the new component. At present sketch1 is active of newly created Centre Pin. Take the project of edge of the hole. Finish the sketch. Start Extrude command. The sketch profile is automatically selected. In the extents drop down menu, select Between option. Select front face of part and then rear face of the part. Click ok. Change the model colour to Popcorn to distinguish it more clearly. Create a new sketch on the YZ plane of the Centre Pin. Take the project of front edge of the Centre Pin. Activate Slice Graphic Command from the Right click context menu. Draw a Three Point Rectangle, coincident with the midpoint and end point of the projected line. Apply a horizontal dimension of 0.03125 in. on the rectangle. Draw a Thee Point Arc inside the rectangle. Finish the sketch. Start Revolve command, first select the sketch profile and later the axis. Click OK. Start the Mirror Command from the Pattern Panel of the Model Tab. Select Revolve1 feature in the browser bar. Select Mirror Plane button in the Mirror dialogue box, then select XY plane of Centre Pin. Click Ok and return back to the assembly. Change the view of Assembly by using View Cube. Apply an Angle Constraint between Part1 and Part2, to show the motion in the Assembly of ‘Hinge’. Activate an Angle Constraint, first select the top face of Par1, then top face Part2, at last select the front face Part2. Click OK. Set the browser Assembly View to Modelling View
Combination Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 22 Combination Pliers-Inventor Studio-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the animation of the ‘Combination Pliers’. Click the following link to get the model file: –http://bit.ly/2n4Yhig Transcription of Video Display of motion in ‘Combination Pliers’ through Inventor Studio Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Combination Pliers-Inventor Studio’. Select Place component from the marking menu and place the ‘Part1’ in the Assembly. Re-orient the model in the design window by using View Cube. Set the current view as Home View by using the toggle next to View Cube. Select the Part1 in the design window and remove its ‘Grounded’ position from the context menu. Apply an Axis Mate between Z Axis of Assembly and Z Axis of Part1. Apply a Mate Constraint between Centre Point of Assembly and Centre Point of Part1. Place the ‘Part2’ in the Assembly. Select the edge of small hole on Part2 to activate Assemble Tool. Then select the edge of small hole on Part1, click green check mark to place Insert Mate between Part2 and Part1. Activate an Angle Constraint, first Select face of Jaw of Part1, and then select YZ Plane of Assembly and in the end select top face of Part1. Click OK. Activate Angle Constraint once again, first Select face of Jaw of Part2, and then select YZ Plane of Assembly and in the end select top face of Part2. Enter the value 180 degree in the Angle Input box and Click Ok. Place the ‘Rivet’ in the Assembly. Select the inner circular edge of Rivet to activate Assemble Tool. Then select the inner small circular edge of hole on the Part2, click green check mark to place Insert Mate between Part2 and Rivet. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select ‘Angle:2’ under the Constraints folder in the Browser Bar, Right click and choose ‘Suppress’ from the context menu. Select Part1 and Part2 in the Browser Bar, right click and choose ‘Contact Set’ from the context menu. Select ‘Activate Contact Solver’ in the Interference panel of Inspect Tab. Drag the Part2, it will stop at the point of Collision between Part1 and Part2. Measure the swing angle between the jaw of Part1 and Part2. The detected swing angle is 40.18 degree. Restore the settings to previous state. Click the ‘Inventor Studio’ icon from the Begin Panel of Environments Tab. Select ‘Angle:1’ Constraint under Part1 in the Browser Bar, right click and select Animate Constraints in the context menu. In ‘Action’ section, enter the value -20.09 degree in the End input box. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box. Click Acceleration Tab. Select ‘Constant Speed’ radio button in the Velocity Profile. Click OK. Select Expand Action Editor Button on the Animation Timeline. Select Angle:1 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu. Edit Mirrored animation action in the Animation Timeline. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box, to give effect of 3 second pause. Click OK. Select ‘Angle:2’ Constraint under Part2 in the Browser Bar, right click and select Animate Constraints in the context menu. In ‘Action’ section, enter the value (180+20.09) degree in the End input box. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 10 second in the End input box. Click Acceleration Tab. Select ‘Constant Speed’ radio button in the Velocity Profile. Click OK. Select Angle:2 constraint in the Animation Timeline, right click and choose ‘Mirror’ from the context menu. Edit Mirrored animation action in the Animation Timeline. In the ‘Time’ section of Animate Constraint dialogue box, enter the value 13 second in the Start input box and enter the value 23 second in the End input box. Click OK. Select Collapse Action Editor Button on the Animation Timeline. Click the Animation Options Button. In the Animation Options dialogue box, click ‘Fit to Current Animation’ button in the ‘Length’ section option. Select Constant Speed radio button in the Default Velocity Profile and click Ok. Clear the screen by activating the Clean Screen command. Click ‘Go to Start’ Button. Click Play Animation button to display motion in Combination Pliers.
