EGR 110 – Inventor Lecture #5

1. EGR 110 – Inventor Lecture #5 • Work Planes • So far we have created sketch planes by: • Selecting an initial sketch plane in the front, top, or right side view • Adding sketch planes to surfaces in existing solids • Sometimes a new feature will be located on a plane that is not available on the current part. In such a case we can add work planes where sketches will be formed in order to add new features. The simplest type of work planes use the standard orthographic planes. We will later see other types of work planes and/or work features. • XY, YZ, and XZ Work Planes • Many features can be developed on standard planes in the world coordinate system. • These planes go through the origin, so it is helpful to have a key point in your model located at the origin. • XY Plane – a plane parallel to the front view • YZ Plane – a plane parallel to the right side view • ZX Plane - a plane parallel to the top view

2. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side as shown below. A work plane will be used to draw the hole. Work plane 2D Sketch: Create the pipe by drawing two concentric circles with their centers at the origin Extrude: Use an extrusion to form the pipe Select Origin as center of circles

3. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) Make the right (YZ) plane visible: Expand (+) Origin in the model browser. As you pause over each plane it will can be seen on the screen. Right-click on YZ plane and turn on () Visibility.

4. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) Add a 2D Sketch to the YZ plane: Select Create 2D Sketch and pick this plane Before adding the 2D sketch After adding the 2D sketch

5. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) • Slice Graphics: • Try to add a circle to the center of the side of the pipe and you will find that youcan’t locate the midpoints or endpoints. This problem can be fixed as follows: • Right-click on the solid and select Slice Graphics. This will remove the portion of the solid in front of the plane so that you will see only the back half of the pipe. The back half of the pipe is now displayed (seen more clearly in the isometric below) Select Slice Graphics

6. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) • Project Geometry: • We still can’t locate the midpoints or endpoints of the pipe to add a circle so we need to use Project Geometry to project some of the pipe features onto the sketch plane. Pick pipe features to project onto the sketch plane (color changes to yellow when selected) Select Project Geometry

7. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) • Draw circle • We can now draw the circle at the center of the side of the pipe. A handy way to center the circle is to locate it at the midpoint of a diagonal construction line that connects endpoints. Diagonal construction line Isometric View

8. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) • Extrude the circle • Note that even through the circle cannot be seen in the view below (as it is inside the pipe), it can still be selected as the Profile. Select circle as Profile

9. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) • Extrude the circle (continued) • Use the following extrusion options: • - Cut • - Symmetric • - Extents: All Cut Symmetric

10. EGR 110 – Inventor Lecture #5 Example: Create a pipe with a hole through the side (continued) Final Result Final Result after turning off Visibility of YZ Plane Final Result

11. EGR 110 – Inventor Lecture #5 Offset Work Planes Work planes can be created which are offset from any desired surface. Example: Create the part shown to the right using a work plane. Make all walls and the bottom of the model 0.125” thick. The basic steps are illustrated below, but are shown in more detail in the following slides. Create basic solid Add sketch plane, slice graphics, and draw rectangle Add offset work plane Extrude (cut) rectangle Final result

12. EGR 110 – Inventor Lecture #5 Example (continued) • Create 2D Sketch of Front View • Extrude to form basic solid (1.25” used in this example)

13. EGR 110 – Inventor Lecture #5 Example (continued) • Add Work Plane • Select Plane on Work Features menu • Select front plane of solid • Hold down left mouse button and slide the plane behind the face • Enter the offset distance (-0.125” in this case)

14. EGR 110 – Inventor Lecture #5 Example (continued) • Add 2D Sketch to work plane just created • Use Slice Graphics to only show solid features behind the plane • Use Project Geometry to project key edges onto the work plane After adding 2D Sketch to Work Plane: After using Slice Graphics Project Geometry used to project key edges onto work plane

15. EGR 110 – Inventor Lecture #5 Example (continued) • Draw rectangle. Use dimensions to control two key distances from edges of solid model. Rectangle and dimensions add to 2D Sketch Isometric view

16. EGR 110 – Inventor Lecture #5 Example (continued) • Extrude the rectangle with the following options: • Select Distance (1.25 – 0.125 – 0.125 = 1.00”) • Direction (behind plane) • Cut Note that all walls and the bottom are 0.125” thick Rectangle extruded to form box to be cut from model

17. EGR 110 – Inventor Lecture #5 Example (continued) Final Result after turning off Visibility of Work Plane Final Result

18. EGR 110 – Inventor Lecture #5 • Features in Inventor • Recall that Inventor models may contain various types of features, including: • Placed Features(no 2D Sketch required): • Holes • Fillets • Threads • Chamfers • Etc • Sketched Features(one or more 2D Sketches required): • Extrusion (based on one 2D Sketch) • Revolution (based on one 2D Sketch) • Sweep (based on two 2D Sketches) – to be covered next

19. EGR 110 – Inventor Lecture #5 • Swept Features • Extrusion – Used to project (or sweep) a profile along a linear path. • Sweep – Used to sweep a profile along any path(a curved path, for example) • A sweep is very useful for creating wires, tubing, etc., that follow some path. • A swept feature in Inventor requires two sketches: • 2D path(along which the profile will be swept) • Profile (created in a plane that is perpendicular to the plane containing the 2D path) Extrusion Sweep Path Extrude profile along a linear path Sweep along a sketched path Profile Profile

20. EGR 110 – Inventor Lecture #5 Example: Create a section of tubing (shown to the right) that follows a curved path using a sweep. • Add a 2D Sketch in the front view and create the following sketch (the required path):

21. EGR 110 – Inventor Lecture #5 Example: Create a section of tubing that follows a curved path using a sweep (continued). • Turn on Visibility for the YZ (right) plane and add a 2D Sketch to this plane. • Select Project Geometry and then select the lower part of the path so that you can tell where it intersects the sketch plane. Select Project Geometry from menu and then pick this line • YZ plane made visible • 2D Sketch added to the YZ plane

22. EGR 110 – Inventor Lecture #5 Example: Create a section of tubing that follows a curved path using a sweep (continued). • Add two circles to form the Profile. The center of the circles must be on the path. If a green dot does not appear then perhaps Project Geometry was not correctly used in the last step. Add circles for Profile. Be sure that the Green Dot appears when locating the centers. Draw circles from the right view Or draw circles from the isometric view

23. EGR 110 – Inventor Lecture #5 Example: Create a section of tubing that follows a curved path using a sweep (continued). • Perform the Sweep • Select Sweep from the 3D Model menu • Select the Profile • Select the Path • Select OK Sweep appears after selecting the Profile and Path. Select OK to accept. Path Profile

24. EGR 110 – Inventor Lecture #5 Example: Create a section of tubing that follows a curved path using a sweep (continued). • Final Result Final Result after turning off Visibility of YZ Plane Final Result

25. EGR 110 – Inventor Lecture #5 Additional examples using sweeps

26. EGR 110 – Inventor Lecture #5 Additional example using a sweep Triple-track window frame

27. EGR 110 – Inventor Lecture #5 Example This simple desk lamp was created using an extrusion, a revolution, and a sweep. Which operation was used for each part? (Discuss and then see next slide for profiles.)

28. EGR 110 – Inventor Lecture #5 Example (continued) Which profiles were used for each operation?