Autodesk Inventor Basic Tutorial || Surfaces

This tutorial covers the basics of surface modelling concepts in ‘Autodesk Inventor’ and provides information about additional detailed learning resources.

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Transcription of Video

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This ‘Inventor Tutorial’ demonstrates how to utilize surface modelling capabilities of the software. Creating models with surfaces is convenient and the result of subsequent features to be created is easy to guess.

Many a time you will find, that the same type of work can be done with the help of solid modelling tools also, but surface modelling has its own importance and benefit.

In this example two closed sketch profiles are visible, that were drawn previously on two different ‘Work Planes’.

Now we will see how to use ‘Boundary Patch Tool’ along with ‘Surface Loft Tool’ to create closed surface bodies.

Later we will see how to join and convert the surface bodies into a solid body by using ‘Sculpt Tool’.

So let us start the tutorial.

Note:-

The video has a little caption assistance, but I have given sufficient amount of pause over the tool and their tip, so that they can be read easily. In addition this, annotations are also applied over important places…. so please focus on them to understand what is being done and how….

1. From the Surface Panel activate Boundary Patch Tool.
2. Create the two surfaces using the displayed closed sketch profiles.
3. Expand this node in the ‘Browser Bar’, here we can see, the software indicates us, that we just created two surface bodies.
4. Activate Loft tool and select the ‘Surface’ in the ‘Output type’ settings, so that we can generate another surface body.
5. So now we have three surface bodies.
6. Next activate Sculpt tool to combine all the three surface, as a result we will get a solid body.
7. On a solid body, we can apply solid modelling features like Fillet, Shell etc., see how…
8. Now activate ‘Half Section View’ to examine the finished component.
9. Our model is complete, see how it would look like, after applying some setting related to lightning and colours which is called rendering.

To learn and practise more about Surface Modelling in Autodesk Inventor please visit the following YouTube Playlist which is updated time to time …..

https://www.youtube.com/playlist?list=PLKWX3xUP3pPr3uAtDu_Hc70NZzq8RJkxh

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Some other links mentioned in the video….

Please visit the following link to know how sketches profiles were create….

https://youtu.be/Po8e8RHXt1I?t=1m5s

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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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Creating a Notch of Mug-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 201

Creating a Notch of Mug-Autodesk Inventor 2013 (with caption and audio narration)

In this exercise, we are using a partially constructed model of ‘Mug-Plastic’. We will take help of 2D&3D sketches, work planes, work points, 3D surfaces by using boundary patch tool and sculpt feature to complete the model.

 

Click the following link to get the model file: - http://bit.ly/2osv0P9

 

 

Transcription of Video

1. Open the file of ‘Mug-Plastic’.
2. At present a surface is visible in the design window which is created with the help of Revolve Tool.
3. Open the visibility of Sketch1 from the browser bar.
4. Create a new work plane on this point, perpendicular to Y Axis of the model.
5. Auto-Resize this work plane.
6. Create a sketch on the newly created Work Plane11.
7. Take the project of XY plane and top circular edge of the model with the help of Project Geometry Tool.
8. Convert all the projected edges into construction geometry.
9. Close the visibility of Sketch1 from the browser bar.
10. Now proceed ahead and draw a triangular shape geometry intact with the projected circular edge of the model.
11. The sketch is complete, so exit from the sketching environment.
12. Create a new work plane, parallel to Work Plane11 at an offset distance of 1.25 inches in downward direction.
13. Close the visibility of Work Plane11.
14. Create a new sketch on Work Plane12.
15. Take the project of the model by using Project Cut Edges tool.
16. And take the project of XY Plane with the help of Project Geometry tool.
17. Finish the 2D sketch.
18. Create a work point at the intersection of this line and circle.
19. In the same manner add three more work points at the vertices of the triangular shaped geometry.
20. Close the visibility of Work Plane12 and Sketch22.
21. Activate ‘New 3D Sketch’ command from the marking menu.
22. Create a 3D Line between Work Point5 and Work Point6.
23. Right click in the graphic window and finish the 3D sketch.
24. In the same way, create a 3D Line between Work Point5 and Work Point7 in a new 3D sketch.
25. At last connect the Work Point8 with the Work Point5 by following the same procedure.
26. Close the visibility of all Work Points.
27. Activate the ‘Boundary Patch’ tool from the Surface Panel of 3D Model Tab.
28. Boundary Patch dialogue is visible in the graphics window.
29. Select two 3D Lines and one edge of triangular shaped geometry for creating a new 3D surface.
30. Click Ok to create the Boundary Patch Feature.
31. Open the visibility of Sketch21 which is hidden under the Boundary Patch Feature.
32. Activate the Boundary Patch Tool once again.
33. This time select the edge of Boundary Patch4 and both visible lines to create another Boundary Feature.
34. Activate the ‘Extend Surface’ tool from the drop down list of Surface panel.
35. Extend Surface dialogue box is visible in the graphics window.
36. Edges selection is active by default.
37. Select this edge of Boundary Patch4 to extend the surface.
38. Leave the value of Extents distance as it is and click Ok to execute the command.
39. In the same manner Extend the other 3D surface created with the help of Boundary Patch5.
40. Close the visibility of Sketch21.
41. Open the visibility of Work Plane11.
42. Activate the ‘Sculpt’ tool from the Surface Panel of 3D Model Tab.
43. Sculpt tool dialogue box is visible in the graphics window.
44. Surfaces selection is active by default.
45. Right click in the graphics window and ‘Select All’ option from the context menu.
46. A preview of sculpt is visible in the graphic window.
47. Click OK to create the Sculpt feature.
48. Sculpt feature combined all the surfaces into a solid body.
49. Close the visibility of Work Plane11 and save the part file.
50. Create a new sketch on the top face of the model.
51. Convert the projected top edge of the model into construction geometry.
52. Duplicate this enclosed profile by using Offset tool.
53. And set the offset distance value 0.125 inch.
54. Exit from the sketching environment.
55. Activate the Extrude command from the marking menu.
56. Enclosed profile is automatically selected in the graphics window.
57. Drag the direction indicator in downward direction.
58. Set the distance value 0.0625 inch on the mini tool bar.
59. Select ‘Join’ operation.
60. Click the green check mark to execute the extrude command.
61. Rotate the model on the back side.
62. Create a new sketch on this face.
63. Duplicate the outer projected edge of the model by offset tool.
64. Enter the offset distance value 0.0625 inch.
65. Finish the 2D Sketch.
66. Extrude this profile 0.1875 inch.
67. Click Home View button over the View Cube.
68. Activate the Shell tool from the Modify panel of 3D Model tab.
69. Shell dialogue box is visible in the graphics window.
70. Remove Faces selection option is activated by default.
71. Select top face of the model to remove it.
72. The preview of shell is visible in the graphics window.
73. Set the Thickness value 0.0625 inch.
74. Click OK to execute the Shell feature.
75. Now the notch of Mug is complete.
76. Inspect the model with the help of ‘Cross Section Analysis’ tool.