Documenting Your Design: Parts List and Balloons

1 Sep, 2003 By: Jeff Wymer

One of the most important functions of assembly drawings is the Bill of Materials (BOM), which lists all of the parts and assemblies required to make up an assembly. A BOM includes items such as number of parts, materials, weights, and descriptions. Balloons identify an item listed in the BOM, and the balloon identifier will correspond to the part/assembly identifier in the BOM. Autodesk Inventor can automate the time-consuming process of creating bill of materials and balloons on your assembly drawings. In this column, we're going to cover how to define a parts list, customize the output to meet your specific needs, and balloon your assembly components.

Creating a Parts List

Once you've created the assembly drawing views required to document your design, you can create a parts list (BOM) from any drawing view. The best way to start is by selecting the Parts List icon from the Drawing Annotation tool palette. Then, you can choose the drawing view you want the parts list created from. The next step is to define the type of numbering system and the options you want to use for your parts list in the dialog box, as shown in Figure 1.

You start by using Level, which sets the type of numbering for the parts list. First Level creates a parts list with subassemblies assigned nested numbering (for example, 3, 3.1, 3.1.1). You can use Parts Only, which consecutively numbers all parts in the assembly even if they are contained in subassemblies, or Range, which allows you to control the range of components to include in the parts list; however, this choice is not available when First-Level Components is selected. The options available to you include Format, which splits the parts list into columns, and Columns, which sets the number of columns. Picking Left or Right moves the columns respectively when increasing the number of rows. After setting the options, simply select where you want to place the parts list on your drawing sheet.

Figure 1. During the parts list creation you have control over what range of components to be documents and the formatting of the parts list.

The Parts List icon color in the Browser changes to red when one or more parts list entries are outdated. You can update the entire parts list at once using the Browser's Update context menu option. But before you update the entire parts list, you may want to check which entries are outdated or update entries individually. To do this, double-click the parts list icon, and then click the Compare button in the Edit Parts List dialog box. Compare checks the values in the selected parts list against the current properties values of the parts; if the values are different, the corresponding cells are highlighted.

Modifying the Parts List

After you place the parts list, you can change several elements. For instance, you can change the number of columns defined during creation, or you can document non-engineering items such as decals, paint, and so on. This can all be accomplished by editing the parts list. The easiest method is to simply double-click on it. This will launch the Edit Parts List dialog box, as shown in Figure 2.

Figure 2. AutoDesk Inventor gives you the flexibility to modify the output of the parts list through this easy-to-use dialog box.

To display parts inside of an assembly in the parts list, edit it and expand the plus (+) sign beside the assembly. Autodesk Inventor will automatically renumber the parts within the assembly by appending a dot and corresponding number; example 1.1, 1.2, 1.3, and so on. If you expand a subassembly nested within an assembly, Inventor will automatically expand the numbering sequence by another decimal place. You can change the default delimiter between item numbers by editing the Parts List within the Drafting Standards dialog box, this change must occur before creating the parts list.

To insert a custom part to the parts list, use the Add Custom Parts icons in the Edit Parts List dialog box. Note: there are two Add Custom Parts icons: custom part before or after the current highlighted row. If you add the custom part besfore a row, you may need to use the Renumber function in Edit Parts List to renumber the items in sequential order.

Any value in a cell can be overridden in the Parts List by simply double-clicking within the cell and typing in the new information. Overridden values in the parts list will have a yellow background. The next time an update to the parts list occurs, these custom values will be overridden. If you want to keep the custom value from being updated automatically, use the Freeze function. However, freeze will not automatically override any parts list updates. To access the Freeze function, right-mouse click over the highlighted cell and choose the Freeze option; cells that are frozen will appear in magenta.

You may override which columns are displayed in the parts list. By default Autodesk Inventor displays the item number, quantity, part number (this is the file name by default), and the description. The Parts List automatically retrieves these values from the model properties associated to the part and assembly files. To select other columns to be displayed, use the Column Chooser icon from the Edit Parts List dialog box, as shown in Figure 3. You can simply select which columns you want to remove or add to the parts list. Custom properties can be defined at the part and assembly level and retrieved and documented in the parts list automatically. To retrieve custom properties, choose Custom Properties > Model.


To add balloons to your design use the Balloon icon from the Drawing Annotation palette, or use the predefined shortcut key: B. After selecting the component to attach to the balloon, you can now drag the leader location for the balloon and terminate the leader by using the context menu and choosing Continue. Inventor also includes the capability to auto-balloon your design by using the Auto-Balloon function, which requires a selected drawing view to apply all balloons to. You may preselect a set of part edges, and then use the auto-balloon tool to only balloon the pre-selected parts.

Figure 3. The display of information in the parts list is controlled through the Column Chooser dialog box. A simple addition or removal of columns will update the parts list automatically.

Inventor includes alignment functions to allow you to align your balloons either horizontally or vertically. The first balloon selected defines the balloon location you want to align to. You can then select the other required balloons to be aligned, access the context menu, and choose Align and the alignment direction.

You can quickly align existing balloons vertically or horizontally, and optionally space them equally according to an offset distance you specify in the Balloon tab of the Drafting Standards dialog box. To align balloons, select a balloon, hold down CTRL, and select the other balloons to align. The first balloon you select defines the alignment index and will not be moved. All other selected balloons will be moved into alignment with the first one. If you choose an offset option, the spacing between them is automatically adjusted. Otherwise, their aligned position is projected orthographically from their previous location.

You can attach a custom part balloon to an existing balloon. For example, you can attach a balloon for thread-locking cement to an existing balloon for a bolt. To attach a custom part balloon; right-click the existing balloon and select Attach Custom Balloon from the context menu; in the Custom Part dialog box, click the left (gray) column for the desired custom part, select OK; and click a point on the desired side of the existing balloon to position and attach the balloon. Optionally you can drag the custom balloon to position it on different sides of the existing balloon.


Autodesk Inventor automates the tedious and time-consuming process of creating bill of materials and balloons for assembly drawings. Furthermore, Inventor gives you the flexibility to control the output of your parts list and balloons, including being able to document non-designed components such as paint, decals and other custom parts.

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