13. The Bracket part is listed twice using the configuration name because of the way the configurations are set up for the parts. To list the bracket only once using the filename, open the bracket, right-click one of the configuration names in the ConfigurationManager, and select Properties. In the Bill of Materials Options panel, select Document Name from the drop-down list. Do this for the other configuration, as well.

Notice also that the Description field holds the configuration-specific custom property for Description, which is used in the BOM.

14. Toggle back to the drawing (press Ctrl+Tab), select anywhere on the BOM table, and then select Table Properties from the PropertyManager. Expand the Part Configuration Grouping panel, and select the Display all configurations of the same part as one item option. This changes how the bracket displays, as well as the pins.

15. Now add a column to the BOM that calls on an existing custom property that is already in all the parts. Place the cursor over the last column on the right and right-click it. Choose Insert⇒Column Right. This places a new column to the right of the last one and displays a popup menu that enables you to set the column to be driven by a custom property, as shown in Figure 17.21.

16. In the first drop-down selection box, select the Weight custom property. Click the green check mark icon to accept the changes. If the popup menu disappears and you need to get it back, double-click the column header to re-display it.

FIGURE 17.21

Adding a column to the BOM

17. You can save the BOM with the additional column as a BOM template by right-clicking anywhere in the BOM and selecting Save As. You can then set the type to a BOM template and the directory to the library location for BOM templates.

If you would like to compare your results against those in this example, the finished drawing is called BOM Tutorial Finished.slddrw.

Tutorial: Using Hole Tables

This tutorial guides you through creating and changing settings that are common in SolidWorks Hole Tables. Follow these steps:

1. Create a new drawing from the inch B (no views).drwdot template. If you have not created the BOM tutorial, then move the drawing template named inchB.drwdot from the materials on the DVD to your library location for drawing templates. Then create the drawing from the template.

2. Click the Model View button on the Drawings toolbar, and browse to the part named Hole Table Part.sldprt.

3. Place a Front view and project a Left view and an isometric view. Then press Esc to quit the command. Finally, delete the four pre-defined views.

4. There is not an anchor in this template for a Hole Table, and so if you would like to create one, do this now. Follow the steps in the BOM tutorial for specifying the anchor point.

5. Click the Hole Table button in the Tables toolbar. Figure 17.22 shows a section of the Hole Table PropertyManager with the selections that you need to make for this Hole Table.

6. Once you have completed the selections, click the Next View button at the bottom of the PropertyManager, and make similar selections in the Left view. The holes for both views are added to a single Hole Table.

The table is created using the default settings established in Tools⇒Options⇒Document Properties⇒Tables, but you can change them here for this specific table.

7. Click anywhere in the table, and then select Table Properties at the bottom of the PropertyManager. Changing from numerical to alphabetical assigns a letter to each hole type and a number to each instance of the type. Make this change and update the table. Figure 17.23 shows the table before and after the changes.

8. Change the number of decimal places used in the Hole Table from two places to three.