Animation displayed in ‘Vise’ Assembly–SolidWorks 2017 (with caption and audio narration)
Serial No. 220 Animation displayed in ‘Vise’ Assembly–SolidWorks 2017 (with caption and audio narration) To watch full sketching video of this model ‘Vise’, please visit my another associated video named as ‘Vise’ (Video Tutorial — Volume-1 and 2) SolidWorks. Click the following link to get the model file: – http://bit.ly/2VffJ0i Transcription of the Video Create a new assembly within an English template. The ‘Begin Assembly’ command is already activated in the assembly design window. Browse the ‘Part1’ file from the Vise → ‘Subassembly-1’ folder, here select ‘Part1’ file and open it. Go to the ‘View (Heads-Up)’ toolbar, click on the ‘Visibility Off’ icon. Turn on the ‘View Origins’ button, the assembly origin button will be visible in the assembly design window. Place the ‘Part1’ file over the assembly origin. Now the ‘Part1’ file has fixed in the centre of the assembly. Choose Isometric view. Turn off the ‘View Origins’ button. Save the assembly, name it as ‘Subassembly1’. Activate the ‘Insert Components’ command and place the ‘Part2’ file in the assembly. Apply a ‘Coincident’ mate between the selected face of ‘Part1’ and selected face of ‘Part2’. Apply a ‘Coincident’ mate between the Right Plane of ‘Part1’ & Right Plane of ‘Part2’. Activate the ‘Mate’ command, choose ‘Distance’ option in the ‘Standard Mates’ section. Fill value 5.672 inches in the Distance input box and select the face of ‘Part1’ and select the face of ‘Part2’. Click Ok to apply the Distance mate. Now the ‘Part2’ file is fixed on the base of ‘Part1’, it can’t be moved. Save the subassembly. Place the ‘Part3’ file in the assembly by using ‘Insert Components’ command. Apply a ‘Coincident’ mate between the slotted face of ‘Part1’ and back face of ‘Part3’. Apply a ‘Coincident’ mate between the slotted face of ‘Part1’ & selected face of ‘Part3’ file. Apply a ‘Coincident’ mate between the side face of ‘Part3’ & side face of ‘Part1’ file. Now the ‘Part3’ component is fixed over the slot of ‘Part1’, it can’t rotate or drag it. Go to the ‘Task Pane’ tab, choose the ‘Design Library’ button and select the ‘Toolbox’ icon. Click ‘Add-in now’ button, here more types of ‘component standards’ are available, select one of them according to your choice. Open ‘ANSI Inch’ standard folder, next click ‘Bolts and Screws’ folder. Next click the ‘Countersunk Head’ folder and select ‘Countersunk Bolt’ item. Drag the bolt in graphics area of the assembly as shown. Select 5/16-18 from the Size area and set the length value to 0.875inch. Click OK to accept it and place one more similar bolt, click OK to finish the command. Apply a Concentric mate between the cylindrical face of ‘Countersunk bolt’ & hole of ‘Part3’. Go to the ‘Mates’ folder in the Model Tree, edit the ‘Concentric1’ mate and activate the ‘Lock Rotation’ button to stop the rotation of the bolt. Apply a Coincident mate between the selected face of the bolt and selected face of ‘Part3’. In the same way, fix another countersunk bolt over the second hole of ‘Part3’ by using ‘Mate’ command. Change the colour of bolts ‘Polished Brass’, it looks good. Save the ‘Subassembly1’. Close the ‘Subassembly1’. Create a new assembly file. Browse the ‘Part4’ file in the ‘Subassembly-2’ folder, select ‘Part4’ file and open it. Fix the aforesaid part in the assembly origin as stated in the previous section. Go to the View Cube and choose Isometric View. Activate the ‘Insert Components’ command and place the ‘Part5’ file in the assembly. Apply a ‘Coincident’ mate between the slotted face of ‘Part4’ and back face of ‘Part5’. Apply a ‘Coincident’ mate between the slotted face of ‘Part4’ & selected face of ‘Part5’ file. Apply a ‘Coincident’ mate between the side face of ‘Part5’ & side face of ‘Part4’ file. Save the assembly, name it as ‘Subassembly-2’. Place the two countersunk bolts from the SolidWorks Design Library which was explained earlier. Apply a Concentric mate between the cylindrical face of ‘Countersunk bolt’ & hole of ‘Part5’. Choose ‘Lock Rotation’ option. Apply a Coincident mate between the selected face of the bolt and selected face of ‘Part5’. In the same way, fix another countersunk bolt over the second hole of ‘Part5’ by using ‘Mate’ command. Change the colour of bolts ‘Polished Brass’, it looks good. Close the ‘Subassembly-2’. Create a new assembly file. Browse the ‘Part6’ file in the ‘Subassembly-3’ folder, select ‘Part6’ file and open it. Fix the aforesaid part in the assembly origin. Save the assembly, name it as ‘Subassembly-3’. Place the ‘Handle’ in the assembly. Apply a Concentric mate between the cylindrical face of ‘Handle’ & hole of ‘Part6’. Apply a Coincident mate between the Top Plane of ‘Part6’ and Front Plane of ‘Handle’. Now the Handle is fixed on the ‘Part6’ file, it can’t drag it. Go to the ‘Mates’ folder and edit the ‘Concentric1’ mate, choose ‘Lock Rotation’ option. Click Ok to finish the command. Save the assembly. Place the ‘Spring’ in the assembly. Change the colour of Spring ‘Brushed Aluminum’, it looks good. Go to the ‘View’ tab → select ‘Hide/Show’ button → click on ‘Axes’ icon. Open the visibility of ‘Axis1’ of Spring. Now the ‘Axis1’ of spring is visible in the assembly design window. Apply a Concentric mate between the Axis1 of ‘Spring’ & cylindrical face of ‘Part6’. Apply a Coincident mate between the circular face of ‘Part6’ & selected face of ‘Spring’. Turn-off the ‘Axes’ button. Insert the ‘Washer’ & ‘Pin’ in the assembly. Apply a Concentric mate between the hole of ‘Washer’ & cylindrical face of ‘Part6’. Apply a Coincident mate between the selected face of the Spring and selected face of ‘Washer’. Fix the Pin on the hole of ‘Part6’ by the aid of ‘Mate’ command. Now the subassembly is complete, save and close it. Create a new assembly within an English template. It is a main assembly to create the animation of Vise. Here three subassemblies will be placed which were created earlier. Browse the ‘Subassembly-1’ and open it. Place the ‘Subassembly-1’
