Autodesk Inventor Basic Tutorial - Loft Feature

In this tutorial we would learn about the Loft feature of Autodesk Inventor by developing a solid named Hammer Head.  This feature is used, when we want to create a solid by joining more than one closed profile. Sometimes optional rails and points are used that help in controlling the final outcome.

Addition to this creation process of new Work Planes, Copy/ Paste function of sketches and many more things are displayed.

Click the following link to get the model file: - http://bit.ly/2CcL5Ms






(Tutorial Concept Courtesy – Default SolidWorks Software Help)

Application of ‘Loft’ tool Ex.1-Autodesk Inventor 2013 (with caption and audio narration)

Serial No. 195

Application of ‘Loft’ tool Ex.1-Autodesk Inventor 2013 (with caption and audio narration)

In this exercise, we are using a partially constructed assembly of ‘Grating for Gas Oven’. We will add some 2D sketches, work planes and a loft feature to proceed towards its completion.

 

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

 

 

 

Transcription of Video

1. Open the ‘Grating for Gas Oven’ (.iam) file.
2. Here a pre constructed ‘Part1’ is visible in this Assembly.
3. Activate the ‘Create Component’ tool to create a new part in the Assembly.
4. Select the XY Plane of the assembly as a base plane for the new component.
5. Create a new sketch on the XY Plane of the ‘Part2’.
6. Take the project of Part1 by using ‘Project Cut Edges’ tool.
7. Select the projected model edges in the graphics window and convert them into construction geometry.
8. On the Ribbon, click 'Finish Sketch' icon.
9. Now we will create a new work plane, parallel to YZ Plane of Part2 with the aid of ‘Offset from Plane’ tool.
10. Activate the ‘Offset from Plane’ tool from the Work Features panel of 3D Model tab.
11. Select YZ Plane of ‘Part 2’ from the Browser Bar.
12. Mini toolbar appears in the graphics window.
13. Drag the manipulator arrow button in the graphics window.
14. Enter the offset distance value (-1.875) inch.
15. Click OK to create a new work plane.
16. Create a new sketch on this work plane.
17. Take the project of bottom edge of the Part1 and Y Axis of Part2.
18. Convert both the projected edges into construction geometry.
19. Draw a rectangle of value 0.25 inch X 0.349 inch with the help of ‘Three Point Center Rectangle’ tool.
20. Apply a dimension of 0.2991 inch between center point of rectangle and projected edge of Part1.
21. Finish the 2D Sketch.
22. Create a new work plane parallel to Work Plane1 at an offset distance of 3.25 inch.
23. Close the visibility of Work Plane1.
24. Create a new sketch on Work Plane2.
25. Take the project of top line of previously drawn rectangle.
26. Close the visibility of Sketch1 and Sketch2 from the Browser Bar to clear the screen.
27. Take the project of Y Axis of Part2.
28. Create a new line of 0.4040 inch with the aid of Offset tool.
29. Apply a Coincident Constraint between midpoint of newly created line and projected Y Axis line.
30. Apply 0.59860 inch dimension between these lines.
31. Add two more lines to close the profile.
32. Finish the 2D Sketch.
33. Open the visibility of Sketch2 from the Browser Bar.
34. Activate the ‘Loft’ tool from Create panel of 3D Model tab.
35. Loft dialogue box is visible in the graphics window.
36. On the ‘Curves’ tab, specify the sections to loft.
37. Click under the ‘Sections’ heading and the select both the sketch profiles in the graphics window.
38. Click OK to execute the Loft feature.
39. Close the visibility of Sketch2 and Work Plane2 from the Browser Bar.
40. Change the colour of model to Steel.
41. Return back to the Assembly environment.

Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration)

 

Serial No. 145

Application of 3D sketch with loft feature-Autodesk Inventor 2012 (with caption and audio narration)

In this video, we will describe 3D sketch and its application in the creation of loft feature.

 

Click the following link to get the drawing sheet of the model: http://bit.ly/2m51dLC

 

 

 Transcription of Video

Application of 3D sketch with loft feature

In this video we will describe about 3D sketch and its application in creation of loft feature.

1. This is our sketch which is named Sketch5 in the browser.
2. It is 2 inch up vertically from this point.
3. This sketch is placed on the Work Plane5.
4. Work Plane5 is 4.5 inch away from the Work Plane4.
5. Now we want to connect Sketch5 to the cup of the Spoon like this.
6. For this we will create two 3D sketches.
7. Start a 3D sketch from the Sketch panel of the Model Tab.
8. Create 3D line and close the sketch like this.
9. Once again create another 3D sketch in the same manner.
10. So the required two 3D sketches are in hand which we will use for developing the handle of Spoon.
11. Now pick up the loft tool from the Create panel of the Model Tab and develop the handle of Spoon like this.

Allen Screwdriver

This is the rendering images of our previously created model Allen Screwdriver.

View Full Album

Watch the following video to understand the modelling process of tip of the Allen Screwdriver.

By watching the video the viewer will be able to understand the application of following features / tolls of Autodesk Inventor.

Creating Work Planes
Project Cut Edges (With converting it into construction line)
Circular Pattern
Loft Feature
Placing Component in Assembly
Rotating Component in an Assembly
Assembly Constrains (Mate)
Copy Object
Sculpt(Remove Material)
Interference Analysis

I recommend that viewers should get the finished Part/Assembly associated with the video to easily understand the video. Visit the following link  to get the part file---

Allen Screwdriver (Autodesk Inventor 2010)