Creating Extrusions Using the Sketches
1. In the Model Tree, select Sketch 1.
2. On the
Model tab, click
Extrude from the
Shapes group. The
Extrude tab opens.
3. Click
Options and select
To Next from the
Side 1 and
Side 2 drop-down lists.
4. Click
OK.
5. In the Model Tree, right-click Sketch 1, and click
Show.
6. Ensure that Sketch 1 is not selected in the Model Tree. On the
Model tab, click
Extrude from the
Shapes group. The
Extrude tab opens.
7. Right-click in the graphics window and click
Define Internal Sketch. The
Sketch dialog box opens.
8. Click Use Previous. The Sketch tab opens.
9. On the Graphics toolbar, click
Display Style, and then click
Wireframe.
10. On the Graphics toolbar, click
Datum Display Filters, and clear the
(Select All) check box to clear all datum display check boxes.
11. On the Graphics toolbar, click
Sketch View.
12. On the
Sketch tab, click
Offset from the
Sketching group. The mini toolbar opens.
13. To select a partial loop of curves:
a. In the selection filter at the bottom left of the graphics window, select Curve.
b. Point over the curve at the top of the sketch until it is highlighted. Make sure the tooltip shows Sketch 1. You might need to zoom in and point far to the right on the curve.
c. Click the highlighted curve to select it.
d. On the mini toolbar, click
. The
Chain dialog box opens.
e. Under References, select Rule-based. The curve you selected appears in the Anchor collector.
f. Under Rule, select Partial loop.
g. Click the Extent Reference collector, and point over the curve at the bottom of the sketch until it is highlighted.
h. Click the highlighted curve to select it. A partial loop of orange offset curves appears from the anchor to the extent reference.
| If the partial loop does not go in the direction you intend, click Flip next to Range in the Chain dialog box. |
14. Type –2.7 in the value box, and press ENTER. The negative value switches the offset curves to the other side of the original curves.
15. In the Chain dialog box, click OK. Three orange sketched entities are created.
16. On the mini toolbar, click
.
17. On the
Sketch tab, click
Project from the
Sketching group. The mini toolbar opens.
18. Select the outer vertical line, which is the boundary of the cylinder. A new orange sketched entity is created on the selected edge.
19. On the mini toolbar, click
.
20. On the
Sketch tab, click
Corner from the
Editing group.
a. Click the top angled orange entity, and click the right vertical line. The angled and vertical sketched entities are joined.
b. Click the bottom angled orange entity, and click the right vertical line. A closed box is created.
21. Click
Centerline from the
Sketching group.
a. Click anywhere on the vertical dashed line.
b. Move the pointer. The centerline is attached to the pointer.
c. Click the vertical dashed line again to define the centerline placement.
22. Click
Select from the
Operations group.
23. Hold down left-mouse button and drag a box around the sketched orange lines.
24. Click
Mirror from the
Editing group, and click the vertical centerline.
25. Right-click in the graphics window and choose
Save the sketch and exit.
26. Right-click in the graphics window and choose
Remove Material.
27. In the Extrude tab, do the following:
a. Click the arrow next to
and select
Symmetric from the list.
b. Set the value to
160 and click
OK.
28. On the Graphics toolbar, click
Display Style, and then click
Shading With Edges.
29. On the Graphics toolbar, click
Saved Orientations, and then click
Default Orientation.
30. On the
Model tab, click
Sketch from the
Datum group. The
Sketch dialog box opens.
31. In the Sketch dialog box, do the following:
a. Select the datum plane RIGHT.
b. Click the Reference box and select the inside bottom surface of the piston as shown in following figure.
c. Select Top from the Orientation list and click Sketch.
32. Right-click in the graphics window and click References. The References dialog box opens.
33. Select the datum plane PIN_PLN. The datum plane name appears in the box.
34. Click Close to close the References dialog box.
35. On the Graphics toolbar, click
Sketch View.
36. Click
Centerline from the
Sketching group.
a. Click anywhere on the vertical dashed line to define the start of the centerline.
b. Move the pointer and click the vertical dashed line again to finish defining the vertical centerline placement.
37. Click
Rectangle from the
Sketching group.
a. Click anywhere on the bottom horizontal dashed line to define the start point of the rectangle.
b. Drag the pointer up to the second horizontal line.
c. Continue to drag the pointer to the other side of the vertical centerline.
d. Click again when the rectangle snaps to indicate vertical symmetry. Two arrows appear to signify symmetry.
38. Middle-click to exit the draw rectangle tool.
39. Double-click to edit the width dimension value to 28 and press ENTER.
40. Click
Center and Point from the
Sketching group.
a. Click the intersection of the vertical centerline and upper horizontal dashed line to start the circle.
b. Drag the pointer and click again when the circle snaps to the upper vertical sketched vertices of the rectangle.
41. Click
Delete Segment from the
Editing group.
42. Press CTRL and click lines 1, 2, 3, and, 4 as shown in the following figure.
43. Middle-click to exit the delete segment tool.
44. Right-click in the graphics window and click
Save the sketch and exit.
45. Select Sketch 2 in the Model Tree or in the graphics window.
46. On the
Model tab, click
Extrude from the
Shapes group. The
Extrude tab opens.
47. Click
Options and select
To Next from the
Side 1 and
Side 2 drop-down list.
48. Click
OK.
49. In the Model Tree, select Sketch 2, and click
Extrude. The
Extrude tab opens.
Remove Material is automatically selected.
50. On the
Extrude tab, click the arrow next to
, and click
Symmetric .
51. Edit the value to 28.7 and press ENTER.
52. Click
OK.