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
- Make a new part.
- Select the Revolved Base feature on the Front Plane.
- Draw the cross-section of a goblet.
- Select the midline as the axis of revolution and complete the feature.
- Apply a large fillet to the spot where the stem meets the cup.
- Apply smaller fillets to other edges, as desired.
LOFT and SHELL
- Make a new part.
- Switch to the Sketch tab and click on "Sketch" to create a naked sketch; put your sketch on the Top Plane.
- Draw a hexagon centered on the origin.
- Give the top line of the hexagon the Horizontal property.
- Dimension the hexagon to a 2 inch diameter.
- Exit the sketch.
- Switch to the Features tab.
- Under Reference Geometry, make a new plane.
- Open the feature tree in the main window to reveal the existing planes.
- Specify that your plane is relative to the Top Plane, with an offset of 6 inches.
- Click OK to complete the plane.
- Go to the Sketch tab.
- Click on your new Plane 1.
- Click on the Sketch button to make a new sketch on Plane 1.
- Draw a hexagon centered on the origin, concentric with but larger than the earlier one.
- Give the matching edge the Horizontal property.
- Dimension the hexagon to a 5 inch diameter.
- Exit the sketch.
- Go back to the Features tab and notice that Lofted Base is un-grayed.
- Select Lofted Base.
- In the Profiles box, click on the top left point in each of your two sketches.
- Click OK to complete the loft.
- Click on Shell in the Features tab.
- Click on the large hexagon face.
- Click OK to complete the shell.
- Right click on Plane1 in the feature manager tree and select Hide.
- Color the Loft feature, not the whole part.
- Color the Shell feature a different color.
- Click on the Section View button and drag the arrow.
- Click OK to complete the section view.
- Click the Section View button again to return to a normal view.
- Save your part as Vase.SLDPRT.
The Flex Tool: TWIST
- Start with the vase you created in the previous exercise.
- 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".
- Notice that Flex can do four different things: twist, bend, taper, or stretch.
- Click anywhere on the vase.
- Click on the "Twisting" radio button.
- The twist axis is shown as a dashed blue line.
- You can use the triad (three rings) to rotate the twist axis, but
you probably don't want to do this.
- 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.
- Click OK to complete the twist action.
- Edit the feature again and try some other twist values: 180 degrees, and 520 degrees.
The Flex Tool: BEND
- 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
"Customizee"; select the "Commands" tab; click on the "Features" menu
item; and finally, drag the Flex icon onto the Features toolbar. Then
click "OK".
- Click anywhere on the case.
- Select the Bending radio button.
- The bend axis is shown as a dashed red line.
- Move the bottom trim-plane one third of the way up the vase.
- Right click on the Triad and select "Move triad to Plane 1" (the bottom plane).
- Click on the red trim plane and drag it to bend the vase to about 90 degrees.
- Click OK.
- If you get a self-intersection error, move the trim plane down or reduce the bend angle.
More Flex Tool
- Make a new part.
- Create an Extruded Base on the Right Plane.
- Draw a 0.5 inch by 6 inch rectangle.
- Exit the sketch.
- Set the extrude depth to 1 inch and click OK.
- Click on the Flex feature.
- For the Flex Input, click on your part.
- Set the angle to 90 degrees.
- Click OK to complete the flex.
- Make another Flex feature.
- Drag the triad (little blue ball) from the center to about 3/4 of the way long the part.
- Drag one of the trim planes to the center of the part.
- Set the bend angle to -90 degrees.
- Click OK to complete the flex.
- Color the Boss Extrude feature.
- Fillet two adjacent long edges with a 0.25 inch radius.
- Color the fillet feature.
- Apply a shell to a long flat face of the part with thickness 0.05.
- Color the shell feature.
- Save your part as Snoodle.SLDPRT.
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