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

1. Create a new assembly within an English template.
2. The ‘Begin Assembly’ command is already activated in the assembly design window.
3. Browse the ‘Part1’ file from the Vise → ‘Subassembly-1’ folder, here select ‘Part1’ file and open it.
4. Go to the ‘View (Heads-Up)’ toolbar, click on the ‘Visibility Off’ icon.
5. Turn on the ‘View Origins’ button, the assembly origin button will be visible in the assembly design window.
6. Place the ‘Part1’ file over the assembly origin.
7. Now the ‘Part1’ file has fixed in the centre of the assembly.
8. Choose Isometric view.
9. Turn off the ‘View Origins’ button.
10. Save the assembly, name it as ‘Subassembly1’.
11. Activate the ‘Insert Components’ command and place the ‘Part2’ file in the assembly.
12. Apply a ‘Coincident’ mate between the selected face of ‘Part1’ and selected face of ‘Part2’.
13. Apply a ‘Coincident’ mate between the Right Plane of ‘Part1’ & Right Plane of ‘Part2’.
14. Activate the ‘Mate’ command, choose ‘Distance’ option in the ‘Standard Mates’ section.
15. Fill value 5.672 inches in the Distance input box and select the face of ‘Part1’ and select the face of ‘Part2’.
16. Click Ok to apply the Distance mate.
17. Now the ‘Part2’ file is fixed on the base of ‘Part1’, it can’t be moved.
18. Save the subassembly.
19. Place the ‘Part3’ file in the assembly by using ‘Insert Components’ command.
20. Apply a ‘Coincident’ mate between the slotted face of ‘Part1’ and back face of ‘Part3’.
21. Apply a ‘Coincident’ mate between the slotted face of ‘Part1’ & selected face of ‘Part3’ file.
22. Apply a ‘Coincident’ mate between the side face of ‘Part3’ & side face of ‘Part1’ file.
23. Now the ‘Part3’ component is fixed over the slot of ‘Part1’, it can’t rotate or drag it.
24. Go to the ‘Task Pane’ tab, choose the ‘Design Library’ button and select the ‘Toolbox’ icon.
25. Click ‘Add-in now’ button, here more types of ‘component standards’ are available, select one of them according to your choice.
26. Open ‘ANSI Inch’ standard folder, next click ‘Bolts and Screws’ folder.
27. Next click the ‘Countersunk Head’ folder and select ‘Countersunk Bolt’ item.
28. Drag the bolt in graphics area of the assembly as shown.
29. Select 5/16-18 from the Size area and set the length value to 0.875inch.
30. Click OK to accept it and place one more similar bolt, click OK to finish the command.
31. Apply a Concentric mate between the cylindrical face of ‘Countersunk bolt’ & hole of ‘Part3’.
32. 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.
33. Apply a Coincident mate between the selected face of the bolt and selected face of ‘Part3’.
34. In the same way, fix another countersunk bolt over the second hole of ‘Part3’ by using ‘Mate’ command.
35. Change the colour of bolts ‘Polished Brass’, it looks good.
36. Save the ‘Subassembly1’.
37. Close the ‘Subassembly1’.
38. Create a new assembly file.
39. Browse the ‘Part4’ file in the ‘Subassembly-2’ folder, select ‘Part4’ file and open it.
40. Fix the aforesaid part in the assembly origin as stated in the previous section.
41. Go to the View Cube and choose Isometric View.
42. Activate the ‘Insert Components’ command and place the ‘Part5’ file in the assembly.
43. Apply a ‘Coincident’ mate between the slotted face of ‘Part4’ and back face of ‘Part5’.
44. Apply a ‘Coincident’ mate between the slotted face of ‘Part4’ & selected face of ‘Part5’ file.
45. Apply a ‘Coincident’ mate between the side face of ‘Part5’ & side face of ‘Part4’ file.
46. Save the assembly, name it as ‘Subassembly-2’.
47. Place the two countersunk bolts from the SolidWorks Design Library which was explained earlier.
48. Apply a Concentric mate between the cylindrical face of ‘Countersunk bolt’ & hole of ‘Part5’.
49. Choose ‘Lock Rotation’ option.
50. Apply a Coincident mate between the selected face of the bolt and selected face of ‘Part5’.
51. In the same way, fix another countersunk bolt over the second hole of ‘Part5’ by using ‘Mate’ command.
52. Change the colour of bolts ‘Polished Brass’, it looks good.
53. Close the ‘Subassembly-2’.
54. Create a new assembly file.
55. Browse the ‘Part6’ file in the ‘Subassembly-3’ folder, select ‘Part6’ file and open it.
56. Fix the aforesaid part in the assembly origin.
57. Save the assembly, name it as ‘Subassembly-3’.
58. Place the ‘Handle’ in the assembly.
59. Apply a Concentric mate between the cylindrical face of ‘Handle’ & hole of ‘Part6’.
60. Apply a Coincident mate between the Top Plane of ‘Part6’ and Front Plane of ‘Handle’.
61. Now the Handle is fixed on the ‘Part6’ file, it can’t drag it.
62. Go to the ‘Mates’ folder and edit the ‘Concentric1’ mate, choose ‘Lock Rotation’ option.
63. Click Ok to finish the command.
64. Save the assembly.
65. Place the ‘Spring’ in the assembly.
66. Change the colour of Spring ‘Brushed Aluminum’, it looks good.
67. Go to the ‘View’ tab → select ‘Hide/Show’ button → click on ‘Axes’ icon.
68. Open the visibility of ‘Axis1’ of Spring.
69. Now the ‘Axis1’ of spring is visible in the assembly design window.
70. Apply a Concentric mate between the Axis1 of ‘Spring’ & cylindrical face of ‘Part6’.
71. Apply a Coincident mate between the circular face of ‘Part6’ & selected face of ‘Spring’.
72. Turn-off the ‘Axes’ button.
73. Insert the ‘Washer’ & ‘Pin’ in the assembly.
74. Apply a Concentric mate between the hole of ‘Washer’ & cylindrical face of ‘Part6’.
75. Apply a Coincident mate between the selected face of the Spring and selected face of ‘Washer’.
76. Fix the Pin on the hole of ‘Part6’ by the aid of ‘Mate’ command.
77. Now the subassembly is complete, save and close it.
78. Create a new assembly within an English template.
79. It is a main assembly to create the animation of Vise. Here three subassemblies will be placed which were created earlier.
80. Browse the ‘Subassembly-1’ and open it.
81. Place the ‘Subassembly-1’ on the assembly origin.
82. Now the ‘Subassembly-1’ is fixed in the centre of the assembly.
83. Choose Isometric view.
84. Save the assembly, name it as ‘Vise with Animation’.
85. Insert the ‘Subassembly-2’ in the assembly design area.
86. Rotate the ‘Subassembly-2’ in front of ‘SubAssembly-1’ by using ‘Move with Triad’ tool.
87. Apply a Coincident mate between the bed of ‘Subassembly-1’ and the bottom face of ‘Subassembly-2’.
88. Apply a Coincident mate between the Right Plane of ‘Subassembly-1’ and Front Plane of ‘Subassembly-2’.
89. Drag the ‘Subassembly-2’ to see the result, it can run on the bed of ‘Subassembly-1’.
90. Insert the ‘Subassembly-3’ in the assembly design window.
91. Rotate the ‘Subassembly-3’ in front of ‘SubAssembly-1’ by using ‘Move with Triad’ tool.
92. Pick-up the ‘Part6’ & ‘Part2’ from the Model Tree, right-click and choose ‘Isolate’ option.
93. Go to the ‘View’ tab → select ‘Hide/Show’ button → click on ‘Temporary Axes’ icon.
94. Now the Axes of ‘Part6’ & ‘Part2’ are visible in the assembly design window.
95. Activate the ‘Mate’ command, go to the ‘Mechanical Mates’ tab in the Mate dialogue box.
96. Different types of mechanical mates are available here, choose any suitable mate according to need of the design.
97. In this case we have selected ‘Screw’ mate button.
98. Choose ‘Distance/revolution’ option and select the Axis of ‘Part6’ & Axis of ‘Part2’.
99. Fill the value 1/7 inch in the ‘Distance/revolution’ input box, it will be designated by the ‘Mate Selections’ area.
100. Click OK to execute the ‘Screw Mate’ command.
101. Switch-off the ‘Temporary Axes’ button.
102. Disable the ‘Exit Isolate’ button.
103. Apply a Coincident mate between the circular face of ‘Part4’ and circular face of ‘Part6’.
104. Rotate the Handle of Vise to examine the working of ‘Screw Mate’.
105. When the Handle is rotated either in clockwise or anticlockwise direction, the ‘Subassembly-2’ will run closure or farther from the ‘Subassembly-1’.
106. Activate the ‘Mate’ command, choose ‘Distance’ mate button.
107. Set the value at 0 and select Jaw faces of ‘Subassembly-1’ & ‘Subassembly-2’.
108. Click OK to finish the command.
109. Go to the ‘Motion Study1’ tab and expand the animation timeline.
110. Move the timebar at 1.5 second and go to the ‘Mates’ folder.
111. Place a new key adjacent to ‘Distance1’ mate by the aid of ‘Place Key’ command.
112. Move the timebar at 21.5 second and add a new key.
113. Edit the ‘Distance1’ mate key and set the value 1inch in the Modify dialogue box.
114. Click OK to accept it.
115. ‘Subassembly2’ will open from start point 0 to 1 inch and it will consume time from 1.5 sec. to 21.5 sec. (i.e. time taken 20 seconds)
116. Move the timebar at 29.5 second and place the new key.
117. Move the timebar at 49.5 second, copy the ‘Distance1’ mate key and paste it.
118. Now return back ‘Subassembly-2’ from 1 inch to start point 0, in this case time consumed from 29.5 to 49.5 seconds.
119. Close the Mates folder.
120. In the next section of this video, we will create two additional views to see different positions of the ‘Vise’.
121. These saved views will be used next in the animation timeline.
122. Minimize the animation timeline and clear the screen to see full view of the model.
123. Set the position of the model in following way.
124. Choose ‘New View’ button from the ‘Orientation’ dialogue box.
125. A ‘Named View’ dialogue box will be visible in the design window and change its name as ‘View-1’ and click OK.
126. Now ‘View1’ is added in the Orientation dialogue box.
127. In the same manner, rotate the model in opposite side by using View Cube command and save the view name it as ‘View-2’.
128. Save the assembly and return back to full screen view.
129. Expand the animation timeline.
130. Go to the ‘Orientation and Camera Views’ tab, select the ‘Isometric’ key.
131. Select ‘View-1’ from the ‘Orientation’ dialogue box.
132. Select the ‘Isometric’ key, right-click and choose ‘Replace Key’ option.
133. Now the ‘Isometric’ key is replaced from ‘Isometric’ view to ‘View1’ by using ‘Replace Key’ command.
134. Move the timebar at 23 second and place the new key.
135. The ‘View-1’ of the model will be in still position from start point 0 to 23 sec. (i.e. time taken 23 seconds)
136. Move the timebar at 28 second and select ‘View-2’ from the ‘Orientation’ dialogue box.
137. Place the new key, time consumed 5 seconds from ‘View-1’ to ‘View-2’ position.
138. Move the timebar at 51 second and place the new key.
139. The ‘View-2’ of the model will be in still position from 28 to 51 sec. (i.e. time taken 23 seconds).
140. Move the timebar at 56 second, copy the View-1 key and paste it.
141. Time taken 5 seconds to return back in previous position of the model.
142. Move the timebar at 28 second and go to the ‘Subassembly-1’ folder.
143. Select the ‘Part1’ file and click ‘Add/Update Key’ button.
144. A new key is added at 28 sec. in the animation timeline.
145. Move the timebar at 29.5 second, select the ‘Part1’ file.
146. Activate the ‘Edit Appearance’ command and change the color of ‘Part1’ as reflective green glass.
147. Click OK to accept it.
148. The time is taken 1.5 seconds for change the default color to transparent color of ‘Part1’ file.
149. In the same manner, place two more keys at 49.5 and 51 seconds in the animation timeline.
150. Go to the ‘Subassembly-2’ folder and select ‘Part4’ file.
151. In the same manner, change the color of ‘Part4’ as reflective green glass and add 4 new keys at 28, 29.5, 49.5 & 51 seconds in the animation timeline.
152. Click ‘Calculate’ button to check the animation.
153. Click ‘Stop’ button, now see here the handle of vise is cut in the assembly design area while running of the animation. It’s not good in practice.
154. Now we will create a new View and replace ‘View-2’ by this new view with the help of ‘Replace Key’ command.
155. Set the desired view of the model and develop a new view, name it as ‘View-3’.
156. And replace the key from ‘View-2’ to ‘View-3’ in the animation timeline.
157. In the same way, replace another view key.
158. Finally click calculate button and click ‘Play form Start’ button to observe the animation of ‘Vise’ mechanism.
159. Save the assembly.
160. Return back to the Model view.