Page 130 - Mastering SolidWorks

|
tUtoriaL: Learning to USe Sketch reLationS 99

On the Website
the BibleInchTemplate.prtdot template used in this tutorial is in the chapter 3 folder in the
materials you can download for this chapter from the Wiley website.

1. Create a folder on your hard drive called D:\Library\BibleTemplates. You can put it
where you like, but I recommend a nonsystem drive in a location where it is unlikely to be
overwritten or lost.
2. Go to Tools ➢ Options ➢ File Locations and add a path to the Document Templates list for
the location of the templates folder you just created.
3. Click the New icon. In the New SolidWorks Document dialog box, make sure you see the
Advanced interface. (The button in the lower-left corner should say Novice. If the button
is labeled Advanced, click it to open the Advanced interface.) Click the tab in the interface
that has the name of the new templates folder you just created.
4. Open a new part using the template you just set up.
5. If the planes are showing in the graphics window, turn them off. Go to View ➢ Hide/
Show ➢ Planes. This turns off all planes. If you want to turn off a single plane, right-click
the plane in the graphics window or in the FeatureManager, and select Hide.
6. Select the Front plane in the FeatureManager, and click the Sketch button on the Sketch tab
of the CommandManager (or right-click the plane and select Insert Sketch). Click the Line
tool from the Sketch tab of the CommandManager.
7. Move the cursor near the origin untill the yellow Coincident symbol appears.
8. Draw a line horizontal from the origin. Remember that you can sketch the line in two
ways: Click+click or click-and-drag. Make sure that the line snaps to the horizontal and
that there is a yellow Horizontal relation symbol. The PropertyManager for the line should
show that the line has a Horizontal relation. Also notice that the line is black, but the free
endpoint is blue (after you press Esc to clear the tool). This means that the line is fully
defined except for its length. You can test this by dragging the blue endpoint.

9. Click the Smart Dimension tool on the Sketch toolbar; use it to click the line that you just
drew, and place the dimension. If you are prompted for a dimension, type 1.000. If not,
then double-click the dimension; the Modify dialog box will appear, enabling you to
change the dimension. The setting to prompt for a dimension is found at Tools ➢ Options
➢ General, Input Dimension Value.
10. Draw two more lines to create a right triangle to look like Figure 3.45. If the sketch
relations symbols do not show in the display, turn them on by clicking View ➢ Sketch
Relations. You may want to set up a hotkey for this, because sketch relations are useful
but often get in the way. When you enclose the triangular area, SolidWorks will shade
the triangle if the Shade Sketch Contours is active. This tool is by default on the right
end of the Sketch CommandManager tab.