Solid Edge Beginners Tutorial || Piston

In this video, viewers will learn basic techniques of the Solid Edge ST9 by creating the head of a ‘Piston’. We will use the ordered modelling approach in creating this part.

While creating this model will learn the following topics/tools of the software:--

1. Using the interface of the software.
2. Creating a new part file on the basis of ISO Metric Template.
3. Creating Basic 2D sketches.
4. Application of Drawing, Geometric relationship and various Dimension Tools (especially way to apply diameter dimension using Symmetric Diameter tool) of sketching environment.
5. Extrude Tool.
6. Changing the colour of part using Part Painter.
7. Setting up of lightning and saving them as View Style in the software by using View Overrides command.
8. Creating section Views.
9. Cut Tool.
10. Round Tool.
11. Creating Planes.
12. Mirror Tool.
13. Hole Tool.
14. Revolved Cut Tool.
15. Pattern Tool.

Addition to this there many more things that can be understood by watching the video.

Note:--
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To understand the video easily, focus over places where we have paused our mouse. This is done so as the viewers can easily read the tooltips generated by the software and understand what is being done and why.

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Visit the following link to get the model file… http://bit.ly/2q5zDiK

 

 

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Hem Tool-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 204

Hem Tool-Autodesk Inventor 2013 (with caption and audio narration)

Hem tool is used to strengthen or eliminate sharp edges of the sheet metal face. You can create single, double, rolled and teardrop hems. This tool is available on Create panel of sheet metal Tab.

 

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

 

 

 Transcription of Video

1. Open the Assembly file of ‘Chassis for Constant Voltage Transformer’.

2. In the Browser Bar double click the ‘Part3' file to edit it.

3. Go to the ribbon, Create panel > Hem tool.

4. The Hem dialogue box is visible in the design window.

5. In the Shape tab, the Edge Selection button is active.

6. Select the left inside vertical edge of the sheet.

7. The preview of Hem is displayed in the design window.

8. Fill the values in the ‘Gap’ and ‘Length’ input box as displayed.

9. Click OK to create new hem.

10. Return back to the assembly environment.

11. Mirror of Part3 is automatically updated.

12. In the Browser Bar, double click the ‘Part4' file to edit it.

13. Repeat the same steps and apply two more hem features on the left and right inside vertical edges of the sheet.

14. Reactivate the hem tool and select top inside edge of the sheet.

15. Click more button to expand the dialogue box.

16. By default, ‘Width Extents’ Type ‘Edge’ is selected.

17. Change it to ‘Offset’.

18. In the ‘OffSet1’ input box, expand the node to activate the Measure tool.

19. Select the left face of the sheet and right face of the hem.

20. The distance between the two faces will be added in the offset input box.

21. In the similar way add values in the ‘OffSet2’ input box.

22. Switch to the Bend tab, change the ‘Relief Shape’ type to ‘Tear’.

23. Click OK to execute the command.

24. At the end, remove the remaining extended faces by using Cut tool.

25. Open the Part4 file separately, to check the Flat Pattern of the sheet.

Latch created through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 187

Latch created through Sheet Metal-Autodesk Inventor 2013 (with caption and audio narration)

In this video, the creation of an assembly of the latch is shown. First base body parts of the latch will be created using sheet metal template that will utilize Contour Flange, Cut and Mirror tools. Afterwards, a previously created part Sliding rod will be placed in the assembly to complete it.

 

 

Click the following link to get the model file: – http://bit.ly/2mRK1tf

 

 

 Transcription of Video

Latch created through Sheet Metal (Autodesk Inventor)

1. Open the ‘Latch Body1’ part file.
2. A ‘Base sketch of Latch’ is created in this file.
3. Go on the ribbon > Setup panel > click Sheet Metal Defaults icon.
4. Uncheck the ‘Use Thickness from Rule’ option to specify the thickness value 3/128 inch manually.
5. Go on the ribbon > Create panel > click Contour Flange icon.
6. The Profile selection button is active by default in the Contour Flange dialogue box.
7. Select the sketch profile.
8. A preview of contour flange is visible in the graphics window.
9. The thickness of sheet should be inside of the sketch profile.
10. Set the value 7 7/8 inch in the Distance field.
11. Click OK to create the feature.
12. Create a new sketch on the right face of the part.
13. Take the project of this face by using Project Geometry tool.
14. Convert the projected lines into construction geometry.
15. Draw a rectangle with the given dimensions.
16. Exit from the sketching environment.
17. Go on the ribbon > Modify panel > click Cut icon.
18. The sketch profile will be automatically selected.
19. Choose ‘All’ option under the Extents field.
20. Click OK to apply the cut feature.
21. Create a new sketch on the selected face.
22. Take the project of this edge and convert it to construction geometry.
23. Draw a new line of length 9/16 inch.
24. Apply a coincident constraint between midpoint of the line and midpoint of the projected line.
25. Finish the 2D Sketch.
26. Activate the Contour Flange tool once again.
27. Select the line.
28. Click more button to expand the dialogue box.
29. Set the Width Extents type to ‘Distance’.
30. Enter the value 0.35156 inch in Distance field.
31. Click OK to create the new flange.
32. Go on the ribbon > Pattern panel > click Mirror icon.
33. Select the Contour Flange3 in the graphics window as feature to pattern.
34. Click Mirror Plane button.
35. In the Model browser, pick YZ plane under the Origin folder.
36. Click OK to mirror the feature.
37. Pick the ‘Corner Round’ tool from Modify Panel.
38. And select these four corner edges of the part.
39. In the Corner Round dialogue box, set the radius to 1/64 inch.
40. Click OK to place the fillet.
41. Go on the ribbon > Flat Pattern panel > click Create Flat Pattern icon to generate the flat pattern of the model.
42. Activate the ‘Bend Order Annotation’ tool from the marking menu.
43. The flat pattern will display numbers that represent the order in which the part would be folded.
44. Right click in the graphics window; click OK to finish the bend order annotation command.
45. Double-click the ‘Folded Model’ icon at the top of the Model browser to return to the folded model.
46. Save the part file and close it.
47. Start a new Standard (in) assembly.
48. Place the ‘Latch Body1’ part file by using ‘Place Component’ tool.
49. Save the assembly with the name ‘Latch’.
50. Create a new component using sheet metal template with the name ‘Latch Body2’ in this assembly.
51. Select back face of the Latch Body1 to define the sketch plane for the base feature of the new part.
52. Open the visibility of ‘Base sketch of Latch’ in the Browser Bar.
53. Create a new sketch on this face.
54. Take the project of end points of the sketch and centre point of arc.
55. Close the visibility of ‘Base sketch of Latch’ in the Browser Bar.
56. Recreate the base sketch by joining these projected points.
57. Activate the ‘Sheet Metal Defaults’ command.
58. Uncheck the ‘Use Thickness from Rule’.
59. Set the value 3/128 inch in the Thickness field.
60. Activate the ‘Contour Flange’ tool.
61. And select the sketch profile.
62. Click the ‘Flip Side’ button to set the thickness of sheet inside of the sketch profile.
63. Fill the value 7/8 inch in the ‘Distance’ field.
64. Click OK to create the new flange.
65. Return back to the assembly environment.
66. Save the assembly.
67. Open the ‘Latch Body2’ part file separately.
68. Change the model colour to ‘‘Flaked Reflective - Beige’.
69. Check the Flat Pattern and Bend sequence of the folded sheet.
70. Place the ‘Sliding rod’ in the Assembly.
71. Apply an axis mate between Sliding rod and Latch Body1.
72. Double click the ‘Latch Body1’ in browser bar to edit it.
73. Start a new sketch on this face of the part.
74. Take the project of the face and draw a line connecting the mid points of the projected edges.
75. Convert all the sketches into construction geometry.
76. Create a circle over this line of 1/8 inch diameter that would be 3/8 inch away from the front face of the model.
77. Finish the sketch and start the Cut Tool from modify panel.
78. Select All option in the dropdown of Extents and apply the command.
79. Create 3 more identical holes at an offset distance of 2 3/8 inch between each hole on the same face of the model by using ‘Rectangular Pattern’ tool.
80. Activate Mirror command and duplicate these four holes on the other side of the model.
81. Return back to the assembly and double click the ‘Latch Body2’ to edit it.
82. Create a hole on this face by applying the same procedure as done in the previous part.
83. First create the sketch and then remove the material from the part using Cut feature.
84. Duplicate this hole on the other side of the model by using Mirror command.
85. The fully developed model will look like this.