SolidWorks Intro Part 4

Dave Touretzky

• Up to now we've been restricted to making planar parts using extruded base and extruded cut.
• Let's look at some features that produce three-dimensional shapes.

REVOLVE

1. Make a new part.
2. Select the Revolved Base feature on the Front Plane.
3. Draw the cross-section of a goblet.
4. Select the midline as the axis of revolution and complete the feature.
5. Apply a large fillet to the spot where the stem meets the cup.
6. Apply smaller fillets to other edges, as desired.

LOFT and SHELL

1. Make a new part.
2. Switch to the Sketch tab and click on "Sketch" to create a naked sketch; put your sketch on the Top Plane.
3. Draw a hexagon centered on the origin.
4. Give the top line of the hexagon the Horizontal property.
5. Dimension the hexagon to a 2 inch diameter.
6. Exit the sketch.

7. Switch to the Features tab.
8. Under Reference Geometry, make a new plane.
9. Open the feature tree in the main window to reveal the existing planes.
10. Specify that your plane is relative to the Top Plane, with an offset of 6 inches.
11. Click OK to complete the plane.

12. Go to the Sketch tab.
13. Click on your new Plane 1.
14. Click on the Sketch button to make a new sketch on Plane 1.
15. Draw a hexagon centered on the origin, concentric with but larger than the earlier one.
16. Give the matching edge the Horizontal property.
17. Dimension the hexagon to a 5 inch diameter.
18. Exit the sketch.

19. Go back to the Features tab and notice that Lofted Base is un-grayed.
20. Select Lofted Base.
21. In the Profiles box, click on the top left point in each of your two sketches.
22. Click OK to complete the loft.

23. Click on Shell in the Features tab.
24. Click on the large hexagon face.
25. Click OK to complete the shell.

26. Right click on Plane1 in the feature manager tree and select Hide.

27. Color the Loft feature, not the whole part.
28. Color the Shell feature a different color.

29. Click on the Section View button and drag the arrow.
30. Click OK to complete the section view.
31. Click the Section View button again to return to a normal view.

32. Save your part as Vase.SLDPRT.

The Flex Tool: TWIST

2. Click on the Flex feature in the Features tab.
• If you don't have Flex in your features tab, go to the top pulldown menu and click on Insert, select "Features", and then select "Flex".
3. Notice that Flex can do four different things: twist, bend, taper, or stretch.
4. Click anywhere on the vase.
5. Click on the "Twisting" radio button.
6. The twist axis is shown as a dashed blue line.
7. You can use the triad (three rings) to rotate the twist axis, but you probably don't want to do this.
8. Click on the red trim plane and drag it to apply a twist of about 120 degrees. You can read the twist angle in the parameter box on the left.
9. Click OK to complete the twist action.
10. Edit the feature again and try some other twist values: 180 degrees, and 520 degrees.

The Flex Tool: BEND

1. Create another Flex feature.
• If you don't have Flex in your Features toolbar, you can add it by selecting Tools from the top pulldown menu, then click on "Customize"; select the "Commands" tab; click on the "Features" menu item; and finally, drag the Flex icon onto the Features toolbar. Then click "OK".
2. Click anywhere on the case.
3. Select the Bending radio button.
4. The bend axis is shown as a dashed red line.
5. Move the bottom trim-plane one third of the way up the vase.
6. Right click on the Triad and select "Move triad to Plane 1" (the bottom plane).
7. Click on the red trim plane and drag it to bend the vase to about 75 degrees.
8. Click OK.
9. If you get a self-intersection error, move the trim plane down or reduce the bend angle.

More Flex Tool

1. Make a new part.
2. Create an Extruded Base on the Right Plane.
3. Draw a 0.5 inch by 6 inch rectangle.
4. Exit the sketch.
5. Set the extrude depth to 1 inch and click OK.

6. Click on the Flex feature.
7. For the Flex Input, click on your part.
8. Use the default Bend operation.
9. Set the bend angle to 90 degrees.
10. Click OK to complete the flex.

11. Make another Flex feature.
12. Drag the triad (little white ball) from the center to about 3/4 of the way long the part.
13. Drag one of the trim planes to the center of the part.
14. Set the bend angle to -90 degrees.
15. Click OK to complete the flex.
16. Color the Boss Extrude feature.

18. Color the fillet feature.

19. Apply a shell to a long flat face of the part with thickness 0.05.
20. Color the shell feature.

21. Save your part as Snoodle.SLDPRT.

Embossed Text On A Curved Surface

1. We're going to emboss our initials onto the filleted edge of the Snoodle.
2. Go to the Features tab, and under Reference Geometry, click on Plane.
3. For the first reference, choose the midpoint of the long fillet boundary line; it will show up as an orange dot if you hover right over it.
4. In the "First Reference" section, click on the button for "Create a plane parallel to the screen."
5. Adjust the viewing angle and click the Update Plane button as necessary.
6. Increase the offset value so that the reference plane doesn't intersect the part; it should be just above the surface of the part.
7. Click OK to complete the reference plane.
8. With the plane selected, go to the Sketch tab and click the Sketch button to make a new sketch on that reference plane.
9. Draw a construction line as the baseline for your text.
10. Click on the Text tool.
11. In the Curves box, select the construction line.
12. Type your initials in the Text box.
13. Uncheck the "Use document font" option.
14. Click on the Font button and set the font size to 0.1 inches.
15. Leave the font name as "Century Gothic". Not all fonts work for embossing, but this one does.
16. Click OK to complete the text object.
17. Adjust the line endpoints as necessary to position the text.
18. Exit the sketch.
19. With the new sketch selected, go to the Features tab and click on Extruded Base.
20. Change the Direction1 value from "Blind" to "Up To Surface".
21. Click on the Reverse Direction button to reverse the extrusion direction if necessary.
22. Click on the face of the part we want to extrude up to.
23. Click OK to complete the extrusion.