EGR 110 – Inventor Lecture #9

1. EGR 110 – Inventor Lecture #9 • Section Views • Inventor can easily create section views. Once a base view has been created in a drawing file, additional views can be added, including: • Projected views (orthographic) – used in several previous examples and assignments • Section views (full sections, half sections, aligned sections, etc) • Auxiliary views – typically used to show inclined or oblique surfaces in true shape Why use section views? As discussed in class and in the textbook, section views are often used to more clearly show internal features. Consider the following example which compares the use of a standard projected view with a section view.

2. EGR 110 – Inventor Lecture #9 Example: Comparing projected views and section views Front View (base view) and projected view (Right Side) Front View (base view) and section view (Full Section B-B)

3. EGR 110 – Inventor Lecture #9 • Example 1 – Full Section • Create a wheel (standard inch part) similar to the one shown below. • Use a revolution (draw the profile in the front view) • Add a circular pattern with 6 holes (one located at the top) • The exact dimensions are not critical

4. EGR 110 – Inventor Lecture #9 • Example 1 – Full Section (continued) • Create a drawing file • Use an A-size portrait sheet • Add a base view (use the right side view of the wheel) • Adjust the scale if necessary

5. EGR 110 – Inventor Lecture #9 • Example 1 – Full Section (continued) • Create a full section • Select Section View from the Place Views menu • Specify the cutting-plane line to be used as follows: • Select a circular feature through which the cutting plane will cut • Select a point above the object for the top of the cutting-plane line (with inferred alignment to the center) • Select a point below the object for the bottom of the cutting-plane line • Right-click and select Done Step A Step B Step C

6. EGR 110 – Inventor Lecture #9 • Create a full section (continued) • Move the mouse to the left or right of the cutting plane line and a section view will appear. • Left click to select the desired location of the section view

7. EGR 110 – Inventor Lecture #9 • Create a full section (continued) • The completed full section is now shown below. The label and scale are added automatically to the section view. • Use Tools – Centerline Bisector to add centerlines to the section view • If dashes are missing from the centerlines, adjust the global line scale under Manage – Styles Editor – Standard – Default Standard (ANSI) Note that the section view shows only 2 holes (not 6) of the circular pattern. This follows common standards.

8. EGR 110 – Inventor Lecture #9 • Example 2 – Half Section • Note that the full section used in the last example is symmetric (the top half and the bottom half of the section view are the same). For symmetric objects it is common to use a half section instead of a full section. • Create a wheel – use the same wheel from Example 1 • Create a drawing file - instead of creating a new drawing file, let’s add another sheet to the existing drawing file as follows: • Right-click on the drawing file name and select New Sheet • You can rename the sheets if you wish Original drawing file with one sheet Add a New Sheet Drawing file now shows 2 sheets Rename each sheet if you wish

9. EGR 110 – Inventor Lecture #9 • Example 2 – Half Section (continued) • Create a drawing file (continued) • Select Sheet2 (or Half Section:2 if renamed) and then select Base to add the base view.

10. EGR 110 – Inventor Lecture #9 • Example 2 – Half Section (continued) • Create a half section • Select Section View from the Place Views menu • Specify the cutting-plane line to be used as follows: • Select Point A (use inferred point above the center) • Select Point B (center) • Select Point C (right of center) • Right-click and select Done • Move the mouse to the right and select the location for the section view Point A Point C Point B

11. EGR 110 – Inventor Lecture #9 • Create a half section (continued) • Recall that a centerline should always divide the sectioned and un-sectioned halves of a half section view. To add a centerline: • Right-click on the solid line to be removed and uncheck Visibility • Add a centerline using Annotate – Centerline Bisector Error. Should be a centerline.

12. EGR 110 – Inventor Lecture #9 • Create a half section (continued) • Double-click on the sectioned view to open the Drawing View Window (partially shown to the right). • Change Style from Hidden Lines Removed to Hidden Line • Select OK. Hidden Lines Removed Hidden Line Shaded Error. Hidden lines should be shown.

13. EGR 110 – Inventor Lecture #9 • Create a half section (continued) • The completed half section is shown below (centerline should be added). Error. Hidden lines should not be shown. Right-click on each hidden line and uncheck Visibility.

14. EGR 110 – Inventor Lecture #9 • Add a sectioned isometric • Right-click on the sectioned (right) view and select Projected View. Create a Projected View from the Sectioned View

15. EGR 110 – Inventor Lecture #9 • Add a sectioned isometric (continued) • Add section lines (hatching) to the isometric by right-clicking on the isometric and selecting Edit View. • Select the Display Options tab. • Check the box next to Hatching. Add Hatching to the isometric

16. EGR 110 – Inventor Lecture #9 Example 3 – Revolved Section (or Aligned Section) By now we can see that the key difference in creating a full section and a half section in Inventor is simply how you draw the cutting-plane line. Suppose that we modify the wheel used in the last two examples so that it has 5 holes instead of 6 holes. Neither the full section nor the half section properly describe the wheel. A revolved section is a better choice in this case. Modify the wheel – so that it has 5 holes instead of 6 holes Create a drawing file – or add another sheet to the existing drawing file.

17. EGR 110 – Inventor Lecture #9 • Example 3 – Revolved Section (or Aligned Section) - (continued) • Create the revolved section • Add the base view • Draw the cutting-plane line as shown below. • Note that the section view is created as if the lower hole through which the cutting-plane line passes is revolved into the extreme lower position. • The drawing on the right illustrates the alignment of the holes. Just for illustration.Not part of drawing.

18. EGR 110 – Inventor Lecture #9 • Create the revolved section (continued) • The completed revolved section is shown below (note that centerlines were added.)

19. EGR 110 – Inventor Lecture #9 Example 4 – Offset Section Offset sections are used when normal cutting plane lines miss key features in the object. Create the solid model below – Note that a horizontal cutting-plane line across the middle of the solid would miss the counter-bored holes. Create the drawing file - Add a the base view.

20. EGR 110 – Inventor Lecture #9 Remove these lines • Example 4 – Offset Section - (continued) • Create the Offset Section • Add a cutting-plane line similar to the one shown below. The exact place where the cutting-plane makes a bend through the material is arbitrary, so the corresponding lines in the section view should not be shown. • Remove these lines by right-clicking on them and un-checking Visibility. Arbitrary position for bend

21. EGR 110 – Inventor Lecture #9 • Create the offset section (continued) • The completed offset section is shown below (centerlines added).