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.
Drill Machine-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 30 Drill Machine-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Drill Machine’. Click the following link to get the model file: –http://bit.ly/2ncLp9z Transcription of Video Display of Motion in Drill Machine through Dynamic Simulation Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Drill Machine-Dynamic Simulation’. Select Place component from the marking menu and place the Frame in the Assembly. Place Handle-1 and Handle Cap-1 in the Assembly. Start the Constrain Command and choose Insert Mate from the type option. First select the inner circular edge of Handle Cap, then select outer circular edge of Handle and click Ok. Give another Insert Mate between Inner edge of Handle Cap and circular edge of Frame as displayed. Re-orient the design window using View Cube. Set the current view as Home View using the toggle next to View Cube. Place Gear Wheel and Gear in the Assembly. Apply a Mate Constraint between Axis of Gear Wheel and Axis of Gear. Next, apply a Mate Constraint between face of Gear Wheel and face of Gear. Apply another Mate Constraint between YZ Plane of Gear Wheel and XZ Plane of Gear. Re-orient the Gear Wheel with respect to Frame using Rotate Component Tool. Apply an Axis Mate between Gear Wheel and stud of Frame. Place Spindle in the Assembly. Apply a Mate Constraint between Axis of Frame and Axis of Spindle. Next, apply a Mate Constraint between inner face of supporting cylinder of frame and back face of the spindle. Place Pinion-2 in the Assembly. Apply a Mate Constraint between Axis of Pinion-2 and Axis of Spindle. Apply an Axis Mate between hole on Pinion-2 and hole on Spindle. Place Locking Pin in the Assembly and fix it inside the hole of Pinion using Insert Mate. Place Pinion-1 in the Assembly. Align the Pinion-1 to match it with the Frame. Apply a Mate Constraint between Axis of Frame and Axis of Pinion-1. Select Pinion-1, Pinion-2 and Gear, then right click in the design window, choose ‘Isolate’ from the context menu. Set the Browser from Assembly view to Modeling View. Locate the Intersection Point of Pinion-2 inside the Browser Bar. Apply a Mate Constraint between the Intersection Point of Pinion-2 and Intersection Point of Gear. In the same manner, apply a Mate Constraint between the Intersection Point of Pinion-2 and the Intersection Point of Pinion-1. Activate Motion Constraint; first select the Axis of Pinion-1 and afterward the Axis of Gear. Enter the value 15/56 in the Ratio Input box and click Apply. Apply same step as above to give motion constraint between Pinion-2 and Gear. Right click in the design window, choose Undo Isolate from the context menu. Place Chuck in the Assembly. Apply a Mate Constraint between the Axis of Spindle and the Axis of Chuck. Place a Mate Constraint between inner circular face of Chuck and front face of Spindle. Place another Mate Constraint between YZ Plane of Chuck and YZ Plane of Spindle. Place Three instances of Jaw in the Assembly. Apply an Axis Mate between two subsequent Jaws. Next, apply a Mate between their edges. Apply a Flush Mate between their end faces. In the same manner, constraint the third Jaw. Apply a Mate Constraint between inner circular face of Chuck and rear face of Jaw. Apply a Mate Constraint between the Axis of Chuck and the Axis of Jaw. Place a Mate Constraint between YZ Plane of Chuck and YZ Plane of any one Jaw. Place Handle-2 and Handle Cap-2 in the Assembly. Apply an Insert Mate between inner circular edge of Handle Cap-2 and outer circular edge of Handle-2. Position the Handle Cap-2 in respect of the stud of Frame by using Rotate Component Tool. Apply an Insert Mate between front circular edge of Handle Cap-2 and inner circular edge of stud. Place Handle Connecting Plate in the Assembly. Apply an Insert Mate between edge of the hole on Handle Connecting Plate and inner circular edge of stud. Place Washer-1 in the Assembly. Apply an Insert Mate between edge of the hole on Washer-1 and edge of the hole on Gear Wheel. Apply a Mate Constraint between YZ Plane of Handle Connecting Plate and Axis of the hole on Gear Wheel. Place Screw-2 in the Assembly. Apply an Insert Mate between inner circular edge of Screw-2 and edge of the hole on Handle Connecting Plate. Place Handle-3 and Handle Cap-3 in the Assembly. Fit the Handle Cap-3 over the Handle-3 with the help of Insert Mate. Apply another Insert Mate between the Handle Cap-3 and hole on the Handle Connecting Plate. Place Screw-1 and Nut in the Assembly. Fix the Screw-1 on the Handle-3 with the help of Insert Mate. Fix the Nut on the Screw-1 by applying Insert Mate. Open the Visibility of surfaces named ‘Pitch Diameter’ of Pinion-2, Pinion-1 and Gear. ‘Isolate’ the Pinion-1, Pinion-2 and Gear in the Assembly. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Select Insert Joint in the Marking menu. Select ‘Rolling: Cone on Cone’ from the drop down menu of Insert Joint dialog box. Select Pitch Diameter of Pinion-2 in ‘Component 1’ option and select Pitch diameter of Gear in ‘Component 2’ option and click Apply. In the same manner select Pitch Diameter of Pinion-1 and select Pitch diameter of Gear and click Ok. Finish Dynamic Simulation and return to Assembly Modelling environment. Close the visibility of surfaces named ‘Pitch Diameter’ of Pinion-1, Pinion-2 and Gear. Right Click in the design window and click ‘Undo Isolate’ option. Activate Dynamic Simulation Tool. 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
Vise-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration)
Serial No. 106 Vise-Dynamic Simulation-Autodesk Inventor 2012 (with caption and audio narration) In this video, we will demonstrate how to apply the different type of mates in the assembly environment for creating the Dynamic Simulation of the ‘Vise’. Click the following link to get the model file: – http://bit.ly/2ms77GX Transcription of Video Display of Motion in Vise through Dynamic Simulation Sub Assembly-1: Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Sub Assembly-1’. Select Place component from the marking menu and place the ‘Base Housing’ 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 ‘Part-1’ in the Assembly. Apply a Mate Constraint between the bottom face of Part-1 and inner face of Base Housing. Apply another Mate Constraint between YZ plane of Base Housing and YZ Plane of Part-1. Apply a Flush Mate between front face of Part-1 and front face of Base Housing. Fill the offset value 5.672 inch. Place the ‘Jaw Plate’ in the assembly. Apply a Mate Constraint between slotted face of Base Housing and back face of Jaw Plate. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate. Apply a Flush Mate between the side face of Jaw Plate and side face of Base Housing. Place two identical ‘Screws’ in the Assembly. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate. Save the Sub Assembly-1 and close it. Sub Assembly-2: Create a New Assembly and save it with the name ‘Sub Assembly-2’. Select Place component from the marking menu and place the ‘Sliding Housing’ 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 ‘Jaw Plate’ in the Assembly. Apply a Mate Constraint between slotted face of Sliding Housing and back face of Jaw Plate. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate. Apply a Flush Mate between the side face of Jaw Plate and side face of Sliding Housing. Place two identical ‘Screws’ in the Assembly. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate. Save the Sub Assembly-2 and close it. Sub Assembly-3: Create a New Assembly and save it with the name ‘Sub Assembly-3’. Select Place component from the marking menu and place the ‘Threaded Spindle’ in the Assembly. Place the ‘Compress Spring’ in the Assembly. Apply a Mate Constraint between Y Axis of Compress Spring and Axis of Threaded Spindle. Apply a Mate Constraint between circular face of Threaded Spindle and face of Compress Spring. Place the ‘Washer’ in the Assembly. Apply an Axis Mate between Washer and Threaded Spindle. Apply a Mate Constraint between face of Washer and face of Compress Spring. Place the ‘Pin’ in the Assembly. Apply an Axis Mate between Pin and hole on the Threaded Spindle. Apply a Mate Constraint between XY Plane of Threaded Spindle and YZ Plane of Pin. Place the ‘Handle’ in the Assembly. Apply an Axis Mate between hole on the Threaded Spindle and Handle. Next apply a Mate Constraint between XZ plane of Threaded Spindle and YZ Plane of Handle. Save the Sub Assembly-3 and close it. Main Assembly (Vise): Create a New Assembly and save it with the name ‘Vise-Dynamic Simulation’. Select Place component from the marking menu and place the ‘Sub Assembly-1’ 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 ‘Sub Assembly-2’ in the Assembly. Align the Sub Assembly-2 in front of Sub Assembly-1 by using Rotate Component Tool. Apply a Mate Constraint between the bed of Sub Assembly-1 and bottom face of Sub Assembly-2. Apply a Flush Mate between YZ Plane of Sub Assembly-1 and XY Plane of Sub Assembly-2. Place ‘Sub Assembly-3’ in the Assembly. Apply an Axis Mate between hole on the Sliding Housing and Threaded Spindle. Apply a Mate Constraint between outer rim of hole on Sliding Housing and rear face of Threaded Spindle. Apply a Mate Constraint between subsequent faces of Jaw in the Assembly. Select the previous applied ‘Mate:4’under the Sub Assembly-1 in the Browser Bar, Right click and choose ‘Supress’ from the context menu. Dynamic Simulation 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 Threaded Spindle in ‘Component 1’ selection option and select Circular edge of Part-1 in ‘Component 2’ selection option. Enter the value 1/7 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*7 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 Vise. Change the colour of Vise ‘Green (Clear)’ to watch its motion in transparent view.
Chain-Inventor Studio-Autodesk Inventor 2013 (with caption and audio narration)
Serial N0. 17 In this Autodesk Inventor tutorial, we will learn how to create an animation of chain links similar to what we see in the real world. For this, we will use a chain link (total 61 after duplicating it by using Assembly components pattern tool ) and two sprockets. While creating the animation we will use as well learn various tools and functionalities of the software like basic sketching, creating user-defined work planes and points, utilization of adaptivity features, application of pattern feature along with detailed settings, Assembly Mates, Inventor Studio etc. Video:– Click the following link to get the model file: – http://bit.ly/2n7CS7Q Length of One Chain-Link Loop length of Chain Profile ………………………………………………………………………………… 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 Please check out some more works by us on Autodesk Inventor below– Basic tutorials on Autodesk Inventor by us:—(YouTube Playlist of more than 15 videos.) Detailed tutorials on Autodesk Inventor by us:—(YouTube Playlist of more than 150 videos.) Hope all of you enjoyed the tutorial. If you find the video useful please like it and share it with your friends/colleagues and do not forget to Subscribe us to get latest updates about our new uploads. Click to Subscribe us on YouTube Dear Viewers if you like our work and wanted to support us, to keep continuing the good work, then become a patron of ours at ‘Patreon’ site. Patreon is a simple way for you to contribute to the creator’s work every month/ every time they release their new work and get rewards in return. Please visit the following link to know all about our work and what we are offering as a reward to our patrons… https://www.patreon.com/nisheethsri
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. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘Roller Chain–Dynamic Simulation’. Hold the Ctrl key, and click the Roller Chains tool on the Power Transmission panel of the Design tab. The Roller Chains Generator dialog box will open with its default values. At present ‘Select Chain Mid Plane’ selection is active by default. Select XY Plane of the Assembly. Select first Roller Chain Sprocket 1 pulley in the ‘Sprockets’ section. Click Sprocket properties button to change the sprocket parameters. Enter the value 38 in the ‘Teeth’ input box and click OK. Click OK again. Align the Roller Chain in correct position by using View Cube. Change the color of both the Sprockets from the Browser Bar to watch it more clearly. Select the ‘Chain Drive’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu. Now both the Sprockets 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 ‘Belt’ from the drop down menu of Insert Joint dialog box. 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. 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*3 deg/s and click Ok. In Simulation Player, fill the value 2000 in the Images field area. Clear the screen by activating the Clean Screen command. 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. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘Synchronous Belt–Dynamic Simulation’. Hold the Ctrl key, and click the Synchronous Belts tool on the Power Transmission panel of the Design tab. The Synchronous Belts Component Generator dialog box will open with its default values. At present ‘Belt Mid Plane’ selection is active by default. Select XY Plane of the Assembly. Select first Synchronous pulley in the ‘Pulleys’ section. Click Pulley properties button to change the pulley parameters. Enter the value 38 in the ‘Teeth’ input box and click OK. Select Second Synchronous pulley in the ‘Pulleys’ section. Click Pulley properties button. Enter the value 57 in the ‘Teeth’ input box and click OK. Click OK again. Align the Belt in correct position by using View Cube. Change the colour of both the Pulleys from the Browser Bar to watch it more clearly. Select the ‘Synchronous Belts Transmission’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu. Now both the Pulleys 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 ‘Belt’ from the drop down menu of Insert Joint dialog box. 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. 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*3 deg/s and click Ok. In Simulation Player, fill the value 2000 in the Images field area. Clear the screen by activating the Clean Screen command. 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. Create a New ‘Standard (in) .iam’ assembly and save it with the name ‘V-Belt–Dynamic Simulation’. Hold the Ctrl key, and click the V-Belts tool on the Power Transmission panel of the Design tab. The V-Belts Component Generator dialog box will open with its default values. At present ‘Belt Mid Plane’ selection is active by default. Select XY Plane of the Assembly. Select Second Grooved Pulley in the ‘Pulleys’ section. Click Pulley properties button to change the pulley parameters. In ‘Design Guide’ drop down menu, select Transmission Ratio. Enter the value 1.5 in the Ratio input box. Click OK. Click OK again. Align the Belt in correct position by using View Cube. Change the colour of both the Pulleys from the Browser Bar to watch it more clearly. Select the ‘V-Belts transmission’ Assembly in the Browser Bar and choose ‘Flexible’ in the context menu. Now both the Pulleys 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 ‘Belt’ from the drop down menu of Insert Joint dialog box. 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. 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*3 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 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. Create a ‘New Assembly’ and save it with the name ‘Rack and Pinion-Dynamic Simulation’. 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 deselect Grounded from the context menu. 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 Third select front face of Rack, and click OK. Create a Work Plane in the assembly, coplanar with the base of Rack. Convert this Work Plane to ‘Grounded’ in the Browser Bar. Set the browser from Assembly View to Modeling View using the toggle at the top of the browser. Select Angle:1 Constraint in the Browser under the Constraints folder and Suppress it from the context menu. 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 Planes to make the screen clear. Right click the Mate:6 in the browser and select Supress from the context menu. 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. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Select Insert Joint in the Marking menu. Select ‘Rolling: Cylinder on Plane’ from the drop down menu of Insert Joint dialog box. Select Rolling constraint option. 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. 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 (-575) 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 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) ……………………………………………………… 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 Create a ‘New Assembly’ and save it with the name ‘Worm Gear–Dynamic Simulation’. Select Place component from the marking menu and place the Worm in the Assembly. Select the Worm in the Design window, right click and deselect Grounded from the context menu. At present there are six Degrees of Freedom in Worm and it can be moved in any direction in the Assembly. 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. Apply another Mate Constraint between Centre Point of the Assembly and Centre Point of the Worm. Now only one Degree of Freedom is left and Worm can be moved only on its X Axis. Select Place component from the marking menu and place the Worm Gear in the Assembly. Align the Worm Gear in correct position by using Rotate Component Tool. 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. Close the visibility of Work Planes to clear the screen. 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 Worm Gear and Pitch Diameter of Worm and then apply a Tangent Mate between them. Apply another Mate Constraint between the Z Axis of Worm Gear and YZ Plane of Assembly. Create a Work Axis in the Assembly, coincident with the axis of surface of Pitch Diameter of Worm Gear. 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 Worm Gear 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 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. 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. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab. Activate Insert Joint from the Marking menu. Select ‘Worm Gear’ from the drop down menu of Insert Joint dialog box. 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. 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*40 deg/s and click Ok. Close the visibility of Pitch diameter of Worm Gear and Worm. 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 Worm and Worm Gear. Note: – The worm gear is always driven by the worm.
