Autodesk Inventor Basic Tutorial 2018 || Sheet Metal || Along with captions and audio narration

In this tutorial, we will learn about basic techniques related to Autodesk Inventor software’s Sheet Metal functionality by creating a model named ‘Cover’.

While creating this model we will learn to utilize various tools related to sheet metal modelling like Contour Flange, Flange, Cut, Face Tool, Fold/Refold, Corner Seam Tool, Flat Pattern, Bend Order Annotation etc.

After creating the model we will create a Drawing sheet of the model. Where we will place Folded as well as Flat Pattern of the model along with Bend Notes.

Video Transcription

1. Start a new Sheet Metal Part file using Metric Template.
2. First, define Sheet Metal Defaults.
3. Make sure that Use Thickness from Rule option is active.
4. Next edit sheet metal rules.
5. Define the sheet metal thickness as 3 mm.
6. Fill the value 1 mm in Bend Radius input box.
7. Click done to save all the changes and close the ‘Sheet Metal Defaults’ dialogue box.
8. Create a sketch on the XY plane along with dimensions and proper constraints in the following way.
9. The sketch is complete and it is a fully constrained sketch so exit from the sketching mode.
10. Activate Contour Flange Tool.
11. Select the sketch as profile and fill the value 75 mm in the distance input box.
12. Click Ok to execute the command.
13. Turn off the model shadow and change the colour of the model as per your wish.
14. Make some changes in the lighting settings to see the model clearly.
15. Now create a new sketch over this face of the model in the following way.
16. Activate the Cut tool it will automatically select sketch as a profile.
17. The depth of cut will be equal to the thickness of the sheet.
18. Click Ok to execute the command.
19. Save the file with the name ‘Cover’.
20. Create a new Work Plane by selecting the following edge and this point.
21. Create a sketch on this plane along with dimensions and proper constraints in the following way.
22. Our sketch is complete so exit from the sketching mode.
23. Turn off the visibility of work plane.
24. Activate Contour Flange Tool.
25. First, select sketch profile and then define edges.
26. Switch to Corner Tab, here Auto Mitering option is already active, fill 0.25 mm value as Miter Gap and execute the command.
27. Activate Mirror Tool.
28. Click on mirror solid option whole solid created up till now will be selected automatically.
29. Next, specify plane for the mirror and execute the command.
30. Create a new plane 15 mm above from this face and create a sketch on this plane in the following way.
31. Activate Face Tool, the profile is selected automatically so define the edge for the bend and execute the command.
32. Mirror this Face feature to the other side of the model.
33. Now activate Flange tool.
34. Define edge for the flange and fill 0° as an angle for the flange.
35. Select offset as Width Extents Type.
36. Fill 19 mm as offset values.
37. Set 20 mm as the distance for the flange and execute the command.
38. Create another sketch over this face of the model in the following way.
39. Activate Fold Tool and specify line for the bend.
40. Flip the direction of the bend.
41. Specify Start of Bend option as Fold Location and execute the command.
42. Activate Unfold Tool.
43. Now, specify the following face as Stationary Reference then select this bends to unfold.
44. Next Click Ok to execute the command.
45. Create a new sketch over this plane in the following way.
46. Activate Cut Tool, you can see the sketch profile is automatically selected for the cut.
47. From here activate Cut Across Bend option and execute the command.
48. Activate Refold Tool.
49. Again, specify Stationary Reference first and then select bend to unfold.
50. Click Ok to execute the command.
51. Now activate Flange Tool and define the edge for it.
52. Fill 75° in flange angle and flip the direction of the flange.
53. Fill 85 mm as Flange length.
54. Specify Bend Position as Outside of base face extents.
55. Switch to Bend tab and fill 0.3 mm values in Relief Width and Relief Depth input box.
56. Click Ok to execute the command.
57. Activate Corner Seam Tool.
58. Select Face /Edge Distance option for this Seam feature.
59. Next select edges for the seam.
60. Activate no overlap option.
61. Fill 0.1 mm value in the Gap input box and execute the command.
62. Oh! Here seems to be some mismatching that needs to be corrected.
63. Edit this feature and change the Offset Direction of this Contour Flange in the following way.
64. Now it is quite perfect.
65. Activate Flat Pattern Tool.
66. Here activate Bend Order Annotation command which defines bends sequences of the flat pattern.
67. By clicking on a Glyph we can edit its number.
68. Click Ok and exit the command.
69. We can manually measure the extents of the sheet or we can check it through Flat Pattern Extents dialogue box.
70. Righ click Flat Pattern in the browser bar and activate Flat Patter Extents Command.
71. Close this dialogue box.
72. Create a new Drawing file using Metric Template.
73. First of all, we will change the size of our drawing sheet in the following way.
74. Activate Base View Command.
75. It has automatically selected ‘Cover’ Model file to place on which we were working.
76. Select Flat Pattern in the Sheet Metal View.
77. Set the View scale to .75 and View Style to Hidden Line Removed.
78. Click Ok to execute the command.
79. Next place another Base View.
80. This time we will place Folded Model.
81. Set the orientation of the model to Isometric view using view cube and execute the command.
82. Switch to Annotate tab and activate Bend Notes Tool.
83. Select all the centerline of bends.
84. You can see bend notes are generated and placed side by of centerlines.
85. Click OK to terminate the command.
86. Switch to Manage tab and activate Styles Editor command.
87. Here increase the height of the Annotation Text and save the changes.
88. Delete unnecessary bend notes.
89. Change the position of some bend notes in the following way so that they can easily be recognized and understood.
90. Turn on the Label Visibility of both views.
91. Our work is complete hence save the file.
92. This is final View of our Drawing Sheet.

Visit the following link to get the model file…
http://bit.ly/2q1k3Vu

 

 

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Visit the following link to watch Sheet Metal tutorial on Autodesk Inventor by us

https://www.youtube.com/playlist?list=PLKWX3xUP3pPrzu8lASNE9Ol3n7nxlJLG1

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Visit the following link to watch basic tutorial on Autodesk Inventor by us

https://www.youtube.com/playlist?list=PLb-IhKRMYSERYpB48aY-sZ10fN6CfXIL4

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To watch detailed tutorials on the same software visit the following link

https://www.youtube.com/playlist?list=PL74BDF7431ED13443

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