Animation displayed in 'Pipe Wrench' Assembly--SolidWorks 2014 (with caption and audio narration)

Serial No. 35

Animation displayed in 'Pipe Wrench' Assembly--SolidWorks 2014 (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.
..................................................................................
To watch full sketching video of this model 'Pipe Wrench', please visit on my another associated video named as 'Pipe Wrench' (Video Tutorial) SolidWorks.

Click the following link to get the model file: - http://bit.ly/2VlqBK7

Transcription of the Video

1. Create a new assembly inside an English template.
2. The ‘Begin Assembly’ command is preactivated in the assembly design window.
3. Go to the View tab and turn on the ‘Origins’ button.
4. Place the ‘Part1’ file in the assembly.
5. Turn off the visibility of ‘Origins’ button.
6. Save the file call it as ‘Pipe Wrench with Animation’.
7. When the first part file is placed in the assembly, the part remains as a grounded component.
8. Activate the ‘Insert Components’ command and place the ‘Part2’ file in the assembly.
9. Apply a ‘Concentric’ mate between the two holes of the Part.
10. Apply a ‘Coincident’ mate between the Top Plane of ‘Part1’ and Top Plane of ‘Part2’.
11. Apply an ‘Angle’ mate between these two edges of the parts.
12. Fill the angle value 4.77 degrees in angle input box.
13. Go to the View Cube and select the top view.
14. Now you can examine here, how the angle mate works.
15. Click OK to execute the command.
16. Click the ‘Previous View’ button to return back to the Isometric view.
17. Place the ‘Part5’ file in the assembly.
18. Select the part file and precisely rotate it by using ‘Move with Triad’ command.
19. Apply a ‘Concentric’ mate between inside cylindrical face of ‘Part5’ and hole of ‘Part2’.
20. And choose ‘Lock Rotation’ option to check the movement of the part.
21. Apply a ‘Coincident’ mate between the top face of ‘Part2’ and back face of ‘Part5’.
22. Place the ‘Part6’ and ‘Part7’ file in the assembly.
23. Apply a ‘Coincident’ mate between the top face of ‘Part7’ and side face of ‘Part1’.
24. Apply a ‘Concentric’ mate between hole of ‘Part1’ and hole of ‘Part7’.
25. Apply a ‘Coincident’ mate between the Top Plane of ‘Part1’ and Plane1 of ‘Part7’.
26. Apply a ‘Concentric’ mate between the cylindrical face of ‘Part6’ and inner cylindrical face of hole of ‘Part7’.
27. Apply a ‘Coincident’ mate between the side face of ‘Part7’ and back face of ‘Part6’.
28. Place the ‘Part8’ file in the assembly.
29. And rotate the part to a suitable position.
30. Apply a ‘Concentric’ mate between holes of ‘Part8’ and ‘Part1’.
31. Apply a ‘Coincident’ mate between the side face of ‘Part1’ and back face of the ‘Part8’.
32. Apply a ‘Coincident’ mate between the Top Plane of ‘Part1’ and the Right Plane ‘Part8’.
33. Place a copy of ‘Part6’ file in the assembly and mate it.
34. Place the ‘Part3’ file and rotate in a proper position.
35. Apply a ‘Coincident’ mate between the Top Plane of ‘Part2’ and Front Plane of ‘Part3’.
36. Apply another ‘Coincident’ mate between the Top Plane of ‘Part3’ and Plane3 of ‘Part2’.
37. Place the ‘Part4’ file in the assembly.
38. Apply a ‘Coincident’ mate between the Plane2 of ‘Part2’ and the Right Plane of ‘Part4’.
39. Go to the ‘Mechanical Mates’ tab in the Mate dialogue box.
40. Different types of mechanical mates are available here, choose any mate as you need according to your design.
41. Choose the ‘Screw’ mate button and select the ‘Distance/Revolution’ option.
42. Set the ‘Distance/Revolution’ value 0.205 inches and choose ‘Reverse’ option.
43. And apply the screw mate between Axis1 of ‘Part4’ and Axis1 of ‘Part3’.
44. Click OK to finish the command.
45. Drag the wheel of the wrench to check the screw mate and observe the result.
46. The wheel rotates the jaw of Pipe Wrench with the help of ‘Screw’ mate command.
47. Activate the ‘Move Component’ command and select the ‘Collision Detection’ option.
48. Choose ‘These components’ option and select the ‘Part1’ and ‘Part3’ file.
49. Make sure the ‘Stop at collision’ option should be selected.
50. Activate the ‘Resume Drag’ button and drag the ‘Part3’ file until it touches to the opposite ‘Part1’ file.
51. Now highlighted face shows here to stop the motion of the component at the moment of touch of any other entity.
52. Click OK to finish the command.
53. Apply a ‘Distance’ mate between the side face of ‘Part1’ and side face of ‘Part2’.
54. The ‘Distance’ mate will automatically calculate the distance value of two components.
55. Click OK to finish the command.
56. Click on the ‘Motion Study’ tab and change the position of the model for creating the new view.
57. Activate the ‘View Orientation’ command and select the ‘New View’ option.
58. Set the ‘Named View’ as ‘View-1’ and click OK.
59. Expand the animation timeline and go on the ‘Orientation and Camera’ tab.
60. Right-click on the Orientation and Camera key, choose ‘Replace Key’ option.
61. Now the Orientation and Camera key is replaced by changing from the ‘Isometric’ view to ‘View1’ with the help of ‘Replace Key’ command.
62. Go to the ‘Distance2’ mate and move the timebar at 3 second.
63. Copy the ‘Distance2’ mate key and paste it.
64. Pause the animation for 3 seconds.
65. Move the timebar at 33 second and double click on the distance mate to modify it.
66. Fill the value (1.5831-1.00) inches in the Modify dialogue box and click OK.
67. A new ‘Distance2’ key will be added at 33 second.
68. Move the timebar at 53 second, copy above said key and paste it.
69. A new ‘Distance2’ key will be added at 53 second.
70. Move the timebar at 83 second, copy the ‘Distance2’ mate key and paste it.
71. Go to the ‘Orientation and Camera Views’ tab.
72. Copy the ‘Orientation and Camera Views’ key, whose name is ‘View-1’.
73. Move the timebar at 38 second and paste the ‘View-1’ key.
74. Move the timebar at 48 second and minimize the animation timeline.
75. Go to the View Orientation toolbar and choose ‘Bottom View’.
76. Right-click in the design window and go to the ‘Set Current View As’ option, select ‘Top’ view.
77. Go to the View Orientation toolbar and choose back face of view cube.
78. And set the current view as Front view.
79. Go to the View Orientation toolbar and select this face, it will change into Isometric view.
80. Activate the ‘New View’ and set the ‘Named View’ as ‘View-2’ and click OK.
81. Expand the animation timeline and place the new key.
82. The time consume 10 seconds in changing from View-1 to View-2 position.
83. Copy the ‘View-2’ key and paste the key at 88 second.
84. Move the timebar at 98 second, copy the ‘View1’ key and paste it.
85. Move the timebar at 48 second and Right-click on the ‘Lights, Camera and Scene’ folder.
86. Choose ‘Add Directional Light’ option.
87. Now we will do some changes here in the basic light and light direction.
88. Click OK to execute the command.
89. The ‘Directional5’ light has been added to the Lights folder.
90. Select the ‘Directional5’ light and activate the ‘Add/Update Key’ button.
91. Now the light key is added at 48 second in the animation timeline by using ‘Add/Update Key’ command.
92. In the same manner, add another light key at 38 second in the animation timeline.
93. The time is being taken 10 seconds in changing from Default Light to ‘Directional5’ light to change the light direction of the model.
94. Right-click on the ‘Directional5’ light and choose ‘Off in SolidWorks’ option.
95. Copy the ‘Directional5’ light key and paste the key at 0 second.
96. The Default light remains in still position for 38 seconds.
97. In the same way, place two more ‘Directional5’ light keys at 88 second and 98 second in the animation timeline.
98. Click ‘Calculate’ button and stop the animation.
99. Clear the screen for a full view of the model and save the assembly.
100. Play the animation.
101. Stop the animation, here we have edited on the ‘View1’ position with the help of ‘Update Standards Views’ command.
102. Expand the animation timeline, go on the ‘Orientation and Camera Views’ tab.
103. Minimize the animation timeline and set position of the model.
104. Right-click on the design window and activate the ‘Update Standards Views’ command and select ‘View1’ position.
105. Go to the View Orientation tab and choose ‘View1’ position.
106. Right-click on the ‘Custom’ view key and select ‘Replace Key’ option.
107. In the same manner, update the two more view keys.
108. At the last, click ‘Play from Start’ button to see the animation.

Allen Screwdriver (Solid Edge ST9 Tutorial)

Serial No. 29

Allen Screwdriver (Solid Edge ST9 Tutorial)
In this Solid Edge Tutorial we will describe how to build the model ‘Allen Screwdriver’. The edge of Allen screwdriver has been constructed by different surface tools like Bound, Stitch, Derived etc. It is a Part and Assembly modelling tutorial. This assembly consist 2 part files Screw Driver and Handle that are positioned according to design intent by using Assembly Constraints.
It will cover the following topics.
........................................................................................................
• Creating 2D Sketches on different Planes.
• Use some sketch constraints as Connect, Horizontal/Vertical, and Equal etc. that are applied on during sketch creation.
• Use solid and surface feature command such as Revolved (Surface), Bounded, Stitched, Extrude, Cut, Circular Pattern, Loft, Subtract, Round etc.
• How to patterning an arc and a line by using ‘Derived’ command, this is the easiest way to create a sketch pattern.
• How to create a line by using ‘3D Line’ command in 3D Sketch environment.
• How to create a feature between circle and point by using ‘Loft Protrusion’ command.
• How to change the color of the model by using ‘Part Painter’ tool.
• How to insert component into the assembly using drag and drop from parts library by using ‘Insert Component’ command.
• How to mate the parts by using ‘Flash Fit’ command in the assembly.
• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.
• Use 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 hide all components except the selected components by using ‘Isolate’ command in the assembly.


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

Screw Driver (Solid Edge ST9 Tutorial)

Serial No. 28

Screw Driver (Solid Edge ST9 Tutorial)

In this Solid Edge Tutorial we will describe how to build the model ‘Screw Driver’. The edge of screw driver and handle has been constructed by different surface tools. It is a Part and Assembly modelling tutorial. This assembly consist 2 part files Screw Driver and Handle that are positioned according to design intent by using Assembly Constraints.

It will cover the following topics.

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

• Creating 2D Sketches on different Planes.

• Use some sketch constraints as Connect, Horizontal/Vertical, and Equal etc. that are applied on during sketch creation.

• Use solid and surface feature command such as Revolved (Surface), BlueSurf, Bounded, Stitched, Extrude, Cut, Circular Pattern, Loft, Mirror Copy Feature, Union, Round etc.

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

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

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

• 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.

 

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

Pipe Wrench with Motion Simulation (Solid Edge ST9 Tutorial)

Serial No. 27

Pipe Wrench with Motion Simulation (Solid Edge ST 9 Tutorial)

In this video we will describe you how to animate the assembly of ‘Pipe Wrench’ (Open and Close the Jaw) using ‘Motion’ command. It is assembly modelling tutorial. This assembly consist 1 Assembly and 9 part files (Handle, Jaw, Threading Wheel, 2 rivets, 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 Pipe Wrench mechanism.

It will cover the following topics.

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

• How to set the Screw joint by applying screw pitch (inch per revolution) between two components in motion analysis environment in the assembly.

• How to insert the cylindrical joint between two components.

• How to suppress the mate.

• How to create a custom UCS on the basis of 2D sketch in a part file by using ‘Coordinate System’ command.

• Use assembly commands such as Flash Fit, Axial Align mate, Angle Mate, Connect mate, Mate/Planar Align command etc.

•How to create an Angular relationship between face of two components by applying an angle value (4.77 degree) by using ‘Angle Relationship’ command.

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

• How to flip the component by using ‘Flip Side’ option in ‘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.

 

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

Drill Machine with Animation (Solid Edge ST9 Tutorial)

Serial No. 26

Drill Machine with Animation (Solid Edge ST9 Tutorial)

In this video we will describe you how to animate the assembly of ‘Drill Machine’ with the one bevel gear and two pinion by using ‘Rotational Motor’ command. It is assembly modeling tutorial. This assembly consist 1 Assembly and 22 part files (Drill Machine frame (Multi Body part) Spindle, Drill chuck, Gear, Pinion, Gear hub, Washer, Handle 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 Drill Machine mechanism.

It will cover the following topics.

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

• How to set the motor command between gear and pinion.

• Use assembly commands such as Flash Fit, Axial Align mate, Connect mate, Mate/Planar Align command etc.

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

• How to mating between the vertex point of gear and pinion by using ‘Connect Mate’ command.

• How to create gear relationship between gear and pinion by using ‘Gear’ mate command and how to define the number of teeth of the gear and pinion (15/56) to define the gear interaction.

• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.

• How to flip the component by using ‘Flip Side’ option in ‘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/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.

 

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

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

Pipe Wrench (Volume-1)—Solid Edge ST9 Tutorial

Serial No. 24-A.

Pipe Wrench (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 ‘Pipe Wrench’. It is a Part and Assembly modelling tutorial. This assembly consist 1 Assembly and 9 part files (Handle, Jaw, Threading Wheel with realistic knurling, 2 rivets, 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 Pipe Wrench mechanism.

To watch the video ‘Pipe Wrench (Volume-2)’, how to create a realistic knurling on cylindrical face of the part with the help of ‘Helical Curve’ command in Solid Edge software.

It will cover the following topics.

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

• Creating 2D Sketches on different Planes.

• Use some sketch constraints as Connect, Parallel, Horizontal/Vertical, Equal etc. that are applied on during sketch creation.

• Use features command such as Revolved, Extrude, Cut, Pattern, Helical Cutout, Helical Curve, Rectangular and Circular Pattern, Mirror Copy Feature, Round etc.

• How to create a helical path along the cylindrical face with the ‘Length and Turns’ option by using ‘Helical Curve’ command.

• Use 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 realistic thread in our model Part3 and Part4 (BSP Thread Profile) by sweeping a cross section along a helical path by using ‘Helical Cutout’ command.

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

• Use assembly commands such as Flash Fit, Angle mate, Axial Align mate, Connect mate, Mate/Planar Align command etc.

•How to create an Angular relationship between face of two components by applying an angle value (4.77 degree) by using ‘Angle Relationship’ command.

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

• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.

• How to flip the component by using ‘Flip Side’ option in ‘Flash Fit’ command in the assembly.

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

• Use ‘Show/Hide Component’ option in the assembly to mate the components more easily.

 

Click the following link to get the model file: - http://bit.ly/2ns7jGu

Pipe Wrench (Volume-2)—Solid Edge ST9 Tutorial

Serial No. 24-B.

Pipe Wrench (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 ‘Pipe Wrench’. It is a Part and Assembly modelling tutorial. This assembly consist 1 Assembly and 9 part files (Handle, Jaw, Threading Wheel with realistic knurling, 2 rivets, 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 Pipe Wrench mechanism.

To watch the video ‘Pipe Wrench (Volume-2)’, how to create a realistic knurling on cylindrical face of the part with the help of ‘Helical Curve’ command in Solid Edge software.

It will cover the following topics.

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

• Creating 2D Sketches on different Planes.

• Use some sketch constraints as Connect, Parallel, Horizontal/Vertical, Equal etc. that are applied on during sketch creation.

• Use features command such as Revolved, Extrude, Cut, Pattern, Helical Cutout, Helical Curve, Rectangular and Circular Pattern, Mirror Copy Feature, Round etc.

• How to create a helical path along the cylindrical face with the ‘Length and Turns’ option by using ‘Helical Curve’ command.

• Use 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 realistic thread in our model Part3 and Part4 (BSP Thread Profile) by sweeping a cross section along a helical path by using ‘Helical Cutout’ command.

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

• Use assembly commands such as Flash Fit, Angle mate, Axial Align mate, Connect mate, Mate/Planar Align command etc.

•How to create an Angular relationship between face of two components by applying an angle value (4.77 degree) by using ‘Angle Relationship’ command.

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

• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.

• How to flip the component by using ‘Flip Side’ option in ‘Flash Fit’ command in the assembly.

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

• Use ‘Show/Hide Component’ option in the assembly to mate the components more easily.

Click the following link to get the model file: - http://bit.ly/2ns7jGu

Drill Machine (Volume-1)—Solid Edge ST9 Tutorial

Serial No. 23-A.

Drill Machine (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 ‘Drill Machine’. It is a Part and Assembly modelling tutorial. This assembly consist 1 Assembly and 22 part files (Drill Machine frame (Multi Body part) Spindle, Drill chuck, Gear, Pinion, Gear hub, Washer, Handle 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 Drill Machine mechanism.

How to construct the part ‘Drill Machine Frame’ (Multi body part). After creating the frame convert all multi body parts into a single solid body with the help of ‘Union’ command.

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 Revolved, Extrude, Cut, Subtract, Intersection, Union, Add Body, Normal Cutout, Helical Cutout etc.

• Use the ‘Add Body’ command to create multiple bodies in a single part file (‘Drill Machine Frame’).

• Use the ‘Revolve’ command with different options.

• How to create a realistic thread in our model Spindle and Part1 (UNF Screw External &Internal Thread Profile) 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 commands such as Flash Fit, Axial Align mate, Connect mate, Mate/Planar Align command etc.

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

• How to mating between the vertex point of gear and pinion by using ‘Connect Mate’ command.

• How to create gear relationship between gear and pinion by using ‘Gear’ mate command and how to define the number of teeth of the gear and pinion (15/56) to define the gear interaction.

• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.

• How to flip the component by using ‘Flip Side’ option in ‘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/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.

 

 

Click the following link to get the model file: - http://bit.ly/2LWL8BP

Drill Machine (Volume-2)—Solid Edge ST9 Tutorial

Serial No. 23-B.

Drill Machine (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 ‘Drill Machine’. It is a Part and Assembly modelling tutorial. This assembly consist 1 Assembly and 22 part files (Drill Machine frame (Multi Body part) Spindle, Drill chuck, Gear, Pinion, Gear hub, Washer, Handle 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 Drill Machine mechanism.

How to construct the part ‘Drill Machine Frame’ (Multi body part). After creating the frame convert all multi body parts into a single solid body with the help of ‘Union’ command.

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 Revolved, Extrude, Cut, Subtract, Intersection, Union, Add Body, Normal Cutout, Helical Cutout etc.

• Use the ‘Add Body’ command to create multiple bodies in a single part file (‘Drill Machine Frame’).

• Use the ‘Revolve’ command with different options.

• How to create a realistic thread in our model Spindle and Part1 (UNF Screw External &Internal Thread Profile) 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 commands such as Flash Fit, Axial Align mate, Connect mate, Mate/Planar Align command etc.

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

• How to mating between the vertex point of gear and pinion by using ‘Connect Mate’ command.

• How to create gear relationship between gear and pinion by using ‘Gear’ mate command and how to define the number of teeth of the gear and pinion (15/56) to define the gear interaction.

• How to lock the rotation of the component by using ‘Lock Rotation’ option in ‘Flash Fit’ command in the assembly.

• How to flip the component by using ‘Flip Side’ option in ‘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/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.

 

Click the following link to get the model file: - http://bit.ly/2LWL8BP

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

Nose Pliers (Solid Edge ST9 Tutorial)

Serial No. 14

Nose Pliers (Solid Edge ST9 Tutorial)

In this Solid Edge Tutorial we will describe how to build the model ‘Nose Pliers’. It is a part and assembly modelling tutorial.

It will cover the following topics.

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

• Creating 2D Sketches on different Planes/model faces.

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

• How to project the model edges, curves and sketch elements onto the selected sketch plane by using ‘Project to Sketch’ command.

• Project geometry command is very useful tool for creating the various features to build the part.

• Use features command such as Extrude, Revolved, Swept Cutout, Cut, Chamfer, Round etc.

• Use the ‘Swept Cutout’ command to construct a cutout by extruding a cross section along a path you define.

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

• Check the interface between one another parts by using ‘Check Interference’ command.

• Use 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.

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

 

Click the following link to get the model file: - http://bit.ly/2onMr3G

Combination Pliers (Solid Edge ST9 Tutorial)

Serial No. 12

Combination Pliers (Solid Edge ST9 Tutorial)

In this Solid Edge Tutorial we will describe how to build the model ‘Combination Pliers’. It is a part and assembly modelling tutorial.

It will cover the following topics.

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

• Creating 2D Sketches on different Planes.

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

• How to create Spline between many points for creating a handle of Plier.

• Use features command such as Extrude, Revolved, Loft, Cut, Chamfer, Round 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 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.

 

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

Setting up a Hinge (Pin) Mechanism in Creo Parametric 2.0

Video Tutorial with caption and audio narration
..............................................................................

In this Assembly Modelling Tutorial of Creo Parametric a mechanism of a Hinge is created by using predefined Pin constraint that is available in the software. First of all, the previously created components of Hinge will be placed in the assembly and then mates will be applied to set up the mechanism. To animate this mechanism read a related blog post by me Animation of Hinge || Using Creo Mechanism.

 

Click the following link to get the model file: -http://bit.ly/2nzc29d

 

 

Transcription of Video

1. We have following components of Hinge, which we will place in an assembly.

2. Later we will test its mechanism with the help of Drag Component tool.

3. Create a new assembly with default template.

4. Give it a name Hinge.

5. Place the part_1 in the assembly.

6. Drag the part so that you can see the Datum Planes of Assembly clearly.

7. Constraint Type is set to Automatic by default.

8. Apply a constraint between Right Datum plane of assembly and Right Datum Plane of part_1.

9. Add a new constraint and select Front Datum Planes of assembly and Front Datum Planes of part_1 to apply a coincident constraint automatically.

10. In the same way apply a coincident constraint between Top Datum Plane of Assembly and Top Datum Plane part_1.

11. Now STATUS area indicates that the component is fully constrained in the assembly.

12. Click the green check mark to apply and save the changes.

13. Now place the part_3 in the assembly.

14. Drag the part_3 and re-align it in the graphic window.

15. Select the axis of part_1 and axis of part_3 to apply a coincident constraint between them.

16. Drag the part_3 in the graphics window and apply a coincident constraint between its front datum plane and Front datum plane of the assembly.

17. Now the component is fully constrained in the assembly.

18. Place part_2 in the assembly.

19. Rotate the part and re-align it.

20. Select a predefined constraint named Pin.

21. Select the axis of part_2 and axis of part_3 to apply a coincident constraint between them.

22. Now click the Placement tab and define the reference of translation.

23. The STATUS area indicates the Connection Definition is complete.

24. Click the green check mark to apply and save the changes.

25. Give away different colours to the parts of the assembly so that they can be recognized easily.

26. Align the model in an isometric view using Re-orient tool.

27. Clear the screen by closing the visibility of Datum planes, axis, points and everything else.

28. Select the top face of part_2 and drag it with the help of Drag Component tool to check the mechanism of Hinge assembly.

29. Only part_2 of Hinge can be moved because we applied a pre-defined Pin constraint on it.

30. Re-generate the file and save it.