Inventor Activity 5: Lofted Vase

Transcription

1 Inventor Activity 5: Lofted Vase In this tutorial, you will use a few new commands to create a free form Lofted object. Sometimes you want to create an object that is not made up of square, flat, or perfectly round parts, like a car body, or boat hull. The Loft feature is one way to do that. 1. Open a new Standard (Imperial) part file. 2. On the XZ plane create a sketch of a circle that has a diameter of 1.5 and is centered on the Origin. 3. In the Browser, right click on the XZ plane under Origin and select Visibility. This will allow us to easily use it for other things. 4. Create a new plane, 1.5 above and parallel with the XZ plane. 5. An easy way to do this is to click Start New Sketch, then click and hold the plane you want to offset. Drag the new plane in the direction that you want it and then enter the offset distance. Press the Enter key. 6. Draw an Ellipse on the new sketch that is centered on the first circle. Access the Ellipse command through the circle dropdown menu. 7. Make the major axis of the ellipse 1.5 in radius and the minor axis 0.8 in radius (double click the ellipse to place the dimensions). Click Finish Sketch.

2 8. Create another Offset plane 1.5 above the last plane. 9. Create a circle on it that is 1 in diameter. Make sure it is centered with the first two. 10. Drop down the menu underneath the Sweep feature and select Loft. 11. The Loft dialogue box will appear. Click on the Add Section and then select the three sketch objects that you created. 12. Loft creates smooth shapes that transition from sketch section to section. This shape looks pretty good, but we can have more control over the shape by adding Rails. 13. Click Cancel. 14. Create a new sketch on the YZ Plane. The YZ plane should go through the center of the other sketches. 15. Project Geometry of the 3 original sketches onto the new sketch surface so that you can snap onto them.

3 16. Use the Spline Interpolation line tool in the drop down menu under Line and draw a curvy line connecting the outer points of the projected sketches. The lines of the spline must touch the other sketches. Spline creates smooth curved lines that have no constant radius, like an arc or circle. When adding a spline, every point you click will locate another point of the line, and the line will adjust its curve between these points. These points can be adjusted after the spline is created by adjusting the Handles (in Red) 17. Delete the projected lines at the top and bottom. 18. Draw a Line going vertically through the center of the sketch. Select the Line and click on the Centerline option. This will turn the line into a centerline for a Mirror. 19. Use the Mirror command to Mirror the spline on the Centerline. 20. Delete the horizontal projected lines. 21. Click Finish Sketch. 22. Right click and select Visibility for each of the visible Planes on the screen to turn them off.

4 23. You now have some Sections and some Rails to better define the Loft. 24. Use the Loft feature again. Choose the 3 original sketches as the Sections, and choose the new Splines as the Rails. 25. Click OK. 26. Nice! Next you re going to hollow out the inside of the vase and make an access at the top. 27. Click on the Shell feature. 28. Enter 0.05 in as the Thickness and then select the top face of the shape. This hollows out the vessel, and creates an opening where selected. 29. Click OK.

5 30. For the last step we are going to put some lettering on the side of the vase. 31. Create a new plane, offset from the YZ Plane by 0.9 in. 32. Use the Text tool, and write some text on the plane that lines up in view with the vase. 33. Find the Emboss feature which is located in the drop down menu under Sweep. 34. Choose the lettering as the Profile. Enter of Depth of and choose either Emboss from Face or Engrave from Face. 35. Make sure that the arrow is pointing towards the vase and click OK. Emboss Engrave

6 36. Choose a color to make the vase. 37. Well done! This concludes the basic modeling tutorials. There are many, many, more capabilities within Inventor for modeling. It is beyond the scope of this course to introduce you to all of the possibilities, but you can always try them on your own. Scrounge around in the menus and see what kinds of icons there are. There are countless resources to help you figure out some of the more complex ways of 3D modelling. Try new things and don t be afraid to use CTRL-Z (undo).