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.

Hand Vise (Solid Edge ST9 Tutorial)

Serial No. 25

Hand Vise (Solid Edge ST9 Tutorial)
In this Solid Edge Tutorial, we will describe how to build the model named ‘Hand Vise’. It is a Part modelling as well as assembly modelling tutorial. The 'Hand Vise' assembly consist of 7 part files. First of all we will create a base part file, which will be placed into the assembly and afterward four part will be created in context of the assembly in the assembly environment with the help of ‘Create Part In-Place’ command.
By watching the tutorial viewer will learn following topics of the software.
........................................................................................................
• Creating 2D Sketches on different Planes.
• Sketch constraints as Connect, Parallel, Horizontal/Vertical, Equal etc. that are applied on during sketch creation.
• Features command such as Extrude, Loft Protrusion, Revolve, Thread, Swept Protrusion, Cut, and Mirror Copy Feature etc.
• Use of extrude command with From/To Extent option. Sets the feature extent so that the sketch is projected from the sketch plane to another specified surface.
• How to create a feature between two sketch profiles on the part with the help of four rails by using ‘Lofted Protrusion’ command.
• How to set the End Conditions of the loft feature with ‘Tangent Continuous’ option under the Lofted Protrusion - Tangency Control in ‘Lofted Protrusion’ command.
•. How to create a feature between single path and cross section with the help of one rail by using ‘Swept Protrusion’ command.
• Use of the Mirror Copy Feature command to construct a mirror copy of selected features. The copy is associative to the original features. If the original features are changed or deleted, the mirror features update. You cannot directly edit the mirror features.
•. How to create a thread on the cylinder by using ‘Thread’ command.
• How to change the color of the model by using ‘Part Painter’ tool.
• Use of assembly commands such as Insert Component, Create Part In-Place, and Copy sketch, Subtract, Isolate component, etc.
• Use of  the ‘Copy Sketch’ command, how to copy sketches from a source document to a target document within the context of the active assembly.
• Use of the ‘Create Part In-Place’ command can be used to create a new part or subassembly within the context of an assembly,
•How to check the interface between two components by using ‘Check Interference’ command.
• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.
• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.
• How to rotate and moving part by using ‘Drag Component’ command.
• Use of ‘Show/Hide Component’ option in the assembly to mate the components more easily.
• How to hide all components except the selected components by using ‘Isolate’ command in the assembly.
• Use of the ‘Subtract’ command (Boolean) to remove the tool body volume from selected target bodies in the assembly. You can select multiple target bodies and multiple tool bodies.
• How to apply knurl image on the face of the model with the help of ‘Styles’ tool.

 

Click the following link to get the model file: - http://bit.ly/2MrIjYf

Vise (Volume-2)—Solid Edge ST9 Tutorial

Serial No. 21-B.

Vise (Volume-2)—Solid Edge ST9 Tutorial

(Starting design of the model is created in Volume-1)

In this Solid Edge Tutorial we will describe how to build the model ‘Vise’. It is a Part and Assembly modelling tutorial. This assembly consist of 1 Main assembly, 3 Subassemblies and 12 part files (Jaw Plate, threaded stud, Handle, washer, spring etc.) that are positioned according to design intent by using Assembly Constraints. This tutorial will give you a good practice of applying constraints in an assembly and give you an idea of Vise mechanism.

It will cover the following topics.

........................................................................................................

• Creating 2D Sketches on different Planes.

• Use the sketch constraints that are applied on during sketch creation.

•. Use features command such as Extrude, Revolved, Loft, Cut, Chamfer, Round, Text Profile, Mirror, Hole features Revolved Cut etc.

•. ‘Lofted Protrusion’ command constructs a protrusion by fitting through a series of cross sections. You can define the cross sections using profiles drawn within the command, sketches, or edges of existing features. The cross sections must be closed elements.

• How to create a text on the model by using Text Profile command and emboss the text by using Extrude command.

• Use Extrude feature command to extrude a profile along a straight path.

• Use the Hole command to construct threaded holes.

• Use Mirror copy feature command to construct a mirror copy of selected features.

• How to create a realistic thread (Acme Thread) by sweeping a cross section along a helical path by using ‘Helical Cutout’ command.

• How to apply knurl image on the face of the model with the help of ‘Styles’ tool.

• How to change the color of the model by using ‘Part Painter’ tool.

• Use assembly constraints such as Axial Align mate, Planer Align mate, Mate command etc.

• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.

• Use ‘Show Reference Planes’ option in the assembly to mate the components more easily.

• How to use the Planar Align command to apply a relationship between selected parts.

• How to mate the parts by using ‘Flash Fit’ command in the assembly.

• How to rotate and moving part by using ‘Drag Component’ command. 

Click the following link to get the model file: - http://bit.ly/2VniPiY

Vise (Volume-1)—Solid Edge ST9 Tutorial

Serial No. 21-A.

Vise (Volume-1)—Solid Edge ST9 Tutorial
(Rest of the design of the model is completed in Volume-2)

In this Solid Edge Tutorial we will describe how to build the model ‘Vise’. It is a Part and Assembly modelling tutorial. This assembly consist of 1 Main assembly, 3 Subassemblies and 12 part files (Jaw Plate, threaded stud, Handle, washer, spring etc.) that are positioned according to design intent by using Assembly Constraints. This tutorial will give you a good practice of applying constraints in an assembly and give you an idea of Vise mechanism.

It will cover the following topics.

........................................................................................................

• Creating 2D Sketches on different Planes.

• Use the sketch constraints that are applied on during sketch creation.

•. Use features command such as Extrude, Revolved, Loft, Cut, Chamfer, Round, Text Profile, Mirror, Hole features Revolved Cut etc.

•. ‘Lofted Protrusion’ command constructs a protrusion by fitting through a series of cross sections. You can define the cross sections using profiles drawn within the command, sketches, or edges of existing features. The cross sections must be closed elements.

• How to create a text on the model by using Text Profile command and emboss the text by using Extrude command.

• Use Extrude feature command to extrude a profile along a straight path.

• Use the Hole command to construct threaded holes.

• Use Mirror copy feature command to construct a mirror copy of selected features.

• How to create a realistic thread (Acme Thread) by sweeping a cross section along a helical path by using ‘Helical Cutout’ command.

• How to apply knurl image on the face of the model with the help of ‘Styles’ tool.

• How to change the color of the model by using ‘Part Painter’ tool.

• Use assembly constraints such as Axial Align mate, Planer Align mate, Mate command etc.

• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.

• Use ‘Show Reference Planes’ option in the assembly to mate the components more easily.

• How to use the Planar Align command to apply a relationship between selected parts.

• How to mate the parts by using ‘Flash Fit’ command in the assembly.

• How to rotate and moving part by using ‘Drag Component’ command.

 

Click the following link to get the model file: - http://bit.ly/2VniPiY

Vise with Motion Simulation (Solid Edge ST9 Tutorial)

 

Serial No. 22

Vise with Motion Simulation (Solid Edge ST9 Tutorial)

In this video we will describe you how to animate (Open and Close the Jaw) the assembly of ‘Vise’ by using ‘Motion’ command. It is assembly modelling tutorial. This assembly consist of 1 Main assembly, 3 Subassemblies and 12 part files (Jaw Plate, threaded stud, Handle, washer, spring etc.) that are positioned according to design intent by using Assembly Constraints. This tutorial will give you a good practice of applying constraints in an assembly and give you an idea of Vise mechanism.

It will cover the following topics.

........................................................................................................

• How to set the Screw joint by applying screw pitch.

• How to play the animation by using Simulate Motion button.

• How to change the simulation setting player by using Motion Option command .

• How to suppress the mate.

• Use assembly constraints such as Axial Align mate, Planer Align mate, Mate command etc.

• How to mate the parts by using ‘Flash Fit’ command in the assembly.

• How to rotate and moving part by using ‘Drag Component’ command.

• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.

• Use ‘Show Reference Planes’ option in the assembly to mate the components more easily.

• How to use the Planar Align command to apply a relationship between selected parts.

 


 
Click the following link to get the model file: - http://bit.ly/2odfUxj

Vise - Motion Simulation (Video Tutorial) Siemens NX 10

Serial No. 14

Vise - Motion Simulation (Video Tutorial) Siemens NX 10

In this video we will describe, how to simulate the assembly of 'Vise' with different joints,  Slider joint, Cylindrical joint, Screw joint Revolute joint and create a link between three Subassemblies in Motion Simulation Application Environment.

 

 

Click the following link to get the model file: -http://bit.ly/336HZ81

Vise (Volume-1) Video Tutorial--Siemens NX 10

Serial No. 12-A.

Vise (Volume-1) Video Tutorial--Siemens NX 10

 

Click the following link to get the model file: -http://bit.ly/2oiz3Og

Vise (Volume-2) Video Tutorial--Siemens NX 10

Serial No. 12-B.

Vise (Volume-2) Video Tutorial--Siemens NX 10

 

Click the following link to get the model file: -http://bit.ly/2oiz3Og

Hand Vise (SolidWorks 2014Tutorial)

Serial No. 27

Hand Vise (SolidWorks 2014Tutorial)

  

 
 

Click the following link to get the model file: - http://bit.ly/2ovutMb

Vise (Volume-1) SolidWorks 2014 Tutorial

Serial No. 24-A

Vise (Volume-1) SolidWorks 2014 Tutorial 

In this tutorial we will display the creation process of an assembly named 'Vise'.  It will be created by using part modelling /assembly modelling functionality of SolidWorks Software.

The Vise model has three sub-assemblies.  Each assembly is has modelled part as well as Tool Box components or standard parts. The parts are to be created individually not in context or with reference of other parts of the assembly, after wards they are placed into the assembly and by using assembly mates they are fitted according to the design.

So in this way viewers will be able to observe lot of basic sketching and application of different tools in part modelling along with assembly mates.

Exploded view of Sub-assembly-1 of Vise

Exploded view of Sub-assembly-2 of Vise

Exploded view of Sub-assembly-3 of Vise

The next part of the video can be watched on following link..

Vise (Volume-2) Video Tutorial--SolidWorks 2014

The animation of this model can be created by visiting the following link:--

Animation by Precise Positioning Display in Vise (SolidWorks 2014)

If you want to get the newer version of this video, we have uploaded this video with audio narration only One Volume on our YouTube channel.  Please you can watch this video so that you can understand it easily.

Click the following link to get the model file: - http://bit.ly/2os7Fgk

....................................................................................
Visit the following link to watch the basic tutorial on SolidWorks by us
https://www.youtube.com/playlist?list=PLb-IhKRMYSES3Zw3QHmQVqQ-rcFVzgYHy
.........................................................................
To watch more detailed tutorials on the same software visit the following link
https://www.youtube.com/playlist?list=PLKWX3xUP3pPo77gFCyy669sI76qJa5jKw
...................................................................................
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.
http://www.youtube.com/user/nisheethsorjm?sub_confirmation=1
....................................................................................................
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 a reward to our patrons…
https://www.patreon.com/nisheethsri
...................................................................................................................................

Vise (Volume-2) SolidWorks 2014 Tutorial

 

Serial No. 24-B

Vise (Volume-2) SolidWorks 2014 Tutorial

In this tutorial we will display the creation process of an assembly named 'Vise'.  It will be created by using part modelling /assembly modelling functionality of SolidWorks Software.

The Vise model has three sub-assemblies.  Each assembly is has modelled part as well as Tool Box components or standard parts. The parts are to be created individually not in context or with reference of other parts of the assembly, after wards they are placed into the assembly and by using assembly mates they are fitted according to the design.

So in this way viewers will be able to observe lot of basic sketching and application of different tools in part modelling along with assembly mates.

Exploded view of Sub-assembly-1 of Vise

Exploded view of Sub-assembly-2 of Vise

Exploded view of Sub-assembly-3 of Vise

The previous part of the video can be watched on following link..

Vise (Volume-1) Video Tutorial--SolidWorks 2014

The animation of this model can be created by visiting the following link:--

Animation by Precise Positioning Display in Vise (SolidWorks 2014)

If you want to get the newer version of this video, we have uploaded this video with audio narration only One Volume on our YouTube channel.  You can play this video so that you can understand it easily.

Click the following link to get the model file: - http://bit.ly/2os7Fgk

....................................................................................
Visit the following link to watch the basic tutorial on SolidWorks by us
https://www.youtube.com/playlist?list=PLb-IhKRMYSES3Zw3QHmQVqQ-rcFVzgYHy
.........................................................................
To watch more detailed tutorials on the same software visit the following link
https://www.youtube.com/playlist?list=PLKWX3xUP3pPo77gFCyy669sI76qJa5jKw
...................................................................................
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.
http://www.youtube.com/user/nisheethsorjm?sub_confirmation=1
....................................................................................................
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 a reward to our patrons…
https://www.patreon.com/nisheethsri
...................................................................................................................................

Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 191

Application of ‘Extrude’ tool (Join operation) Autodesk Inventor 2013 (with caption and audio narration)

 

  

Click the following link to get the model file: - http://bit.ly/2omKELY

 

 

Transcription of Video

1. Open the Part1 file.
2. A pre constructed sketch1 is visible in the design window.
3. Double click the Sketch1 in the browser bar.
4. Take the Offset of sketch, of the value 1/4 inch inside the enclosed profile.
5. Activate the extrude command from the marking menu.
6. Extrude dialogue box is visible in the design window.
7. The Profile selection button is active by default.
8. Select the profile enclosed by the yellow sketch and enter the distance value 3/8 inch.
9. Click OK to apply the extrude feature.
10. Open the visibility of Sketch1.
11. Activate the Extrude command once again from the Create panel.
12. Select the profile enclosed by the yellow lines and extrude it 1 inch in upward direction.

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:

1. Create a New ‘Standard (in).iam’ Assembly and save it with the name ‘Sub Assembly-1’.
2. Select Place component from the marking menu and place the ‘Base Housing’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Place the ‘Part-1’ in the Assembly.
6. Apply a Mate Constraint between the bottom face of Part-1 and inner face of Base Housing.
7. Apply another Mate Constraint between YZ plane of Base Housing and YZ Plane of Part-1.
8. Apply a Flush Mate between front face of Part-1 and front face of Base Housing.
9. Fill the offset value 5.672 inch.
10. Place the ‘Jaw Plate’ in the assembly.
11. Apply a Mate Constraint between slotted face of Base Housing and back face of Jaw Plate.
12. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate.
13. Apply a Flush Mate between the side face of Jaw Plate and side face of Base Housing.
14. Place two identical ‘Screws’ in the Assembly.
15. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate.
16. Save the Sub Assembly-1 and close it.

Sub Assembly-2:

1. Create a New Assembly and save it with the name ‘Sub Assembly-2’.
2. Select Place component from the marking menu and place the ‘Sliding Housing’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Place the ‘Jaw Plate’ in the Assembly.
6. Apply a Mate Constraint between slotted face of Sliding Housing and back face of Jaw Plate.
7. Next apply a Mate Constraint between lower face of slotted face and bottom Face of Jaw Plate.
8. Apply a Flush Mate between the side face of Jaw Plate and side face of Sliding Housing.
9. Place two identical ‘Screws’ in the Assembly.
10. Fix both the Screws in the holes on Jaw Plate by using the Insert Mate.
11. Save the Sub Assembly-2 and close it.

Sub Assembly-3:

1. Create a New Assembly and save it with the name ‘Sub Assembly-3’.
2. Select Place component from the marking menu and place the ‘Threaded Spindle’ in the Assembly.
3. Place the ‘Compress Spring’ in the Assembly.
4. Apply a Mate Constraint between Y Axis of Compress Spring and Axis of Threaded Spindle.
5. Apply a Mate Constraint between circular face of Threaded Spindle and face of Compress Spring.
6. Place the ‘Washer’ in the Assembly.
7. Apply an Axis Mate between Washer and Threaded Spindle.
8. Apply a Mate Constraint between face of Washer and face of Compress Spring.
9. Place the ‘Pin’ in the Assembly.
10. Apply an Axis Mate between Pin and hole on the Threaded Spindle.
11. Apply a Mate Constraint between XY Plane of Threaded Spindle and YZ Plane of Pin.
12. Place the ‘Handle’ in the Assembly.
13. Apply an Axis Mate between hole on the Threaded Spindle and Handle.
14. Next apply a Mate Constraint between XZ plane of Threaded Spindle and YZ Plane of Handle.
15. Save the Sub Assembly-3 and close it.

Main Assembly (Vise):

1. Create a New Assembly and save it with the name ‘Vise-Dynamic Simulation’.
2. Select Place component from the marking menu and place the ‘Sub Assembly-1’ in the Assembly.
3. Re-orient the model in the design window by using View Cube.
4. Set the current view as Home View by using the toggle next to View Cube.
5. Place ‘Sub Assembly-2’ in the Assembly.
6. Align the Sub Assembly-2 in front of Sub Assembly-1 by using Rotate Component Tool.
7. Apply a Mate Constraint between the bed of Sub Assembly-1 and bottom face of Sub Assembly-2.
8. Apply a Flush Mate between YZ Plane of Sub Assembly-1 and XY Plane of Sub Assembly-2.
9. Place ‘Sub Assembly-3’ in the Assembly.
10. Apply an Axis Mate between hole on the Sliding Housing and Threaded Spindle.
11. Apply a Mate Constraint between outer rim of hole on Sliding Housing and rear face of Threaded Spindle.
12. Apply a Mate Constraint between subsequent faces of Jaw in the Assembly.
13. Select the previous applied ‘Mate:4’under the Sub Assembly-1 in the Browser Bar, Right click and choose ‘Supress’ from the context menu.
14. Dynamic Simulation
15. Activate the Dynamic Simulation Tool from the Begin Panel of Environments Tab.
16. Select Insert Joint in the Marking menu.
17. Select ‘Screw’ from the drop down menu of Insert Joint dialog box.
18. 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.
19. Enter the value 1/7 in the ‘Pitch’ input box. Click OK.
20. Select Revolution:2 joint in the Browser under the Standard Joints folder, right click and select Properties from the context menu.
21. Click dof 1 (R) tab and select Edit imposed motion button and check the Enable imposed motion option.
22. Click the arrow to expand the input choices, and click Constant Value.
23. Enter the value -360*7 deg/s and click OK.
24. In Simulation Player, fill the value 1000 in the Images field area.
25. Clear the screen by activating the Clean Screen command.
26. Click Run in the Simulation Player to display motion in Vise.
27. Change the colour of Vise ‘Green (Clear)’ to watch its motion in transparent view.

Hand Vise (Autodesk Inventor 2012)

Serial No. 43

Hand Vise (Autodesk Inventor 2012)

 

 

Click the following link to get the model file: - http://bit.ly/2nLs3c0