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FIGURE 17.17

Displaying BOM data inside an assembly document

It can be difficult to match the relative scale of the table to the model. To do this, you have to adjust the zoom state of the model until it is fairly small within the screen, and then place the table. After you place the table, the assembly and the table zoom together. Most users avoid this issue by viewing the table in a separate window. Alternately you can use the BOM Scaling box in the Bill of Materials PropertyManager that enables you to scale the BOM without using the previous method, although the previous method still works.

Another type of table that you can use within a 3D model document is the Title Block table, which can be used inside parts and assemblies. You can use Title Block tables in the drawing to fill in information about the part or assembly and at the same time avoid creating a full 2D drawing.

Tutorial: Using BOMs

Rather than having tutorials for every table type, this chapter has tutorials only for the BOM, Hole Table, and Revision Table. You can transfer the skills you use with these types to the other types.

This tutorial guides you through the steps that are necessary to prepare an assembly for the drawing and BOM. Configurations and custom properties are used in this example. Remember that if a drawing view is cross-hatched and you cannot see the geometry, then you may have to press Ctrl+Q to rebuild it. Follow these steps:

1. Begin this tutorial with SolidWorks closed and Windows Explorer open.

2. If you have not already done so, create a folder for a library that is not in your SolidWorks installation folder. Call it D:\Library\ or something similar. Make a folder inside this folder called Drawing Templates. Copy the files from the DVD named inch B.drwdot and inch B (no views).drwdot to this new folder.

3. Launch SolidWorks and choose Tools⇒Options⇒File Locations⇒Document Template. Click the Add button and add the new library path to the list. Shut down SolidWorks and restart it.

4. Open the assembly BOM Assy.sldasm from the DVD.

5. Click the Make Drawing From Part/Assembly button, and make a new drawing of the assembly from the drawing template in the folder created in Steps 2 and 3.

6. Delete the isometric view, and in its place make a new drawing view using the model view labeled “exploded.” If prompted to use true dimensions in an isometric view, click Accept.

7. Edit the sheet format. Right-click the sketch point at the location indicated in Figure 17.18. In the popup menu that appears, select Set as Anchor and then select Bill of Materials.

FIGURE 17.18

Setting the Table Anchor

8. Exit Edit Sheet Format mode by selecting Edit Sheet from the RMB menu.

9. Select the new view and show it in the exploded state (right-click and select Properties⇒Show in Exploded State). Then choose Insert⇒Table⇒Bill of Materials or click the Bill of Materials button in the Tables toolbar. Use the default selections, except in the panels shown in Figure 17.19.

10. Click inside the exploded view, but not on any part geometry, and then select the Autoballoon tool from the Annotations toolbar. Toggle through the available options to see whether any of the possible autoballoon configurations meet your needs. If not, use the standard Balloon tool to select the part and place the balloon. This gives you more control over the attachment points and placement of the balloons.

11. Change the balloon for the short pin to be a circular split-line balloon (do this by clicking the balloon and then switching the style in the PropertyManager). Notice that the quantity appears in the bottom of the balloon. The drawing view and the BOM should now look like Figure 17.20.

Add a second leader to the balloon for the short pin by Ctrl+dragging the attachment point for the first leader from one pin to the other.

FIGURE 17.19

Creating the Bill of Materials

FIGURE 17.20

The drawing view and the BOM after Step 11

12. Notice that several of the parts