Finalizing Your BOM in Altium Designer | Altium Designer 23 用户手册

Using Altium Documentation

Created: August 23, 2022 | Updated: September 2, 2022

Contents

BOM Verification
Generating a BOM
Mapping Design Data into the BOM
Comparing the Current BOM with an Earlier Revision

All Contents

Parent page: BOM Management with ActiveBOM

BOM Verification

ActiveBOM includes a comprehensive set of BOM checks, that is automatically performed each time the BOM is updated.

BOM Status

Each BOM Item is checked for violations and its status is displayed in the BOM Status column. This column is always visible on the right side of the BOM Items list, displaying an icon that indicates that item's status. Note that a BOM Item can fail more than one of the BOM checks, the icon indicates the most severe failure.

BOM Status Icons:

Clear - component has solutions, these solutions have suppliers with sufficient stock, and at least one solution has been ranked.
Warning
Error
Fatal Error

Hover over the icon for a summary of that part's status. Alternatively, enable the display of the detailed BOM Status column to display detailed information. The column can be enabled either via the ActiveBOM Properties panel, which includes a handy search box or by right-clicking in the column header area of the BOM Items list then choosing the Select Columns command.

Configuring the BOM Checks

The BOM Items are automatically checked for:

Violations associated with Design Items: this includes tests such as parts whose BOM parameters do not match the library parameters (ambiguous parameters), and duplicate designators.
Violations associated with Part Choices: this includes tests such as an unranked MPN (system assigned ranking only), no suppliers, or a missed target price.

The severity level (report mode) of each BOM check is configured in the BOM Checks dialog. Click the Gear icon below the BOM Checks detected violations list in the Properties panel to open the dialog.

To essentially disable a specific check, set its Report Mode to No Report.

When connected to an Altium 365 Workspace, note that the 'Component revision state is restricted from use' violation check is not supported with the Altium Designer Standard Subscription. As such, this entry will not be presented in the BOM Checks listing with this level of access to Altium 365.

Filtering the BOM Items List by BOM Status

The Properties panel displays a list of detected BOM check violations that are present in the current BomDoc. Click the Filter icon (as shown below) to filter the main BOM Items list so that it only displays those BOM Items that fail that BOM check. Note that a BOM Item can fail multiple BOM checks.

Click to filter out all BOM Items except those that fail this BOM check. Click the Gear icon to configure the BOM Checks.

Use the Filter feature to quickly identify all BOM Items that fail a specific BOM Check.

Generating a BOM

The BOM can be generated directly from the ActiveBOM editor. Select the Reports » Bill of Materials command to open the Report Manager dialog and generate the BOM.

The Report Manager presents the BOM data as it will be output. From ActiveBOM it is used to configure the output format and select a template.

The Report Manager is the standard BOM output setup dialog, the same dialog that is opened when Bill of Materials is selected from the schematic or PCB editor's Report menu, or when a BOM is configured in an OutputJob.

The Report Manager shares many features with the ActiveBOM interface, simplifying the process of configuring the BOM.
If there is an ActiveBOM document (BomDoc) in the project then the layout settings defined in it, are automatically applied in the Report Manager.
BOM Sets defined in the ActiveBOM document are available, easily switch from one BOM layout to another.
Excel-format files can be generated, without requiring Microsoft Excel^® to be installed (select the Microsoft Excel File (*.xls, *.xlsx) option).

To learn more about configuring the Report Manager, refer to the page BOM Configuration in the Report Manager.

Mapping Design Data into the BOM

Design data can be passed from the board design process into an Excel Bill Of Materials, by including Field and Column declarations in the Excel template that is applied to the BOM during creation.

Fields - Field declarations are used to pass system, document and project parameters into the BOM, such as filenames, quantity, currency, and so on, that need to be displayed once in the BOM. The Field declaration is replaced by the passed value, as shown in the image below.
Columns - Column declarations are used to pass information that appears in all BOM Items, such as the: designator, description, user-defined parameters, and so on. This can also include line numbers, PCB location data, and custom column data entered into the BomDoc. The Column declaration is replaced by the ColumnName string, with each row below being populated by that column value for a BOM item, as shown in the image below.

Design data mapped into an Excel spreadsheet, by defining them in the Excel template.

To learn more, refer to the Mapping Design Data into the BOM section of the BOM Configuration in the Report Manager page.

Comparing the Current BOM with an Earlier Revision

It's not uncommon for components to change between design releases. To ensure that the process has been completed correctly, many designers like to compare the BOM from the current project with the BOM from a previous revision of the project. If the project is a Workspace project and includes an ActiveBOM BOM document (*.BomDoc), this can be done using the BOM Compare feature.

The BOM Compare report displays what has changed between the current design, and the selected previously released revision. The report can be configured and generated in the following ways:

From an ActiveBOM BomDoc, click Reports » BOM Compare to open the Bom Compare version of the Report Manager dialog. Configure the report as needed then click Export.
From the schematic editor, click Reports » BOM Compare to open the Bom Compare version of the Report Manager dialog. Configure the report as needed then click Export.
From the PCB editor, click Reports » Project Reports » BOM Compare to open the Bom Compare version of the Report Manager dialog. Configure the report as needed then click Export.
From an outjob, right-click on [Add New Report Output] under the Report Outputs entry then choose BOM Compare. To configure the report, right-click on the newly-added BOM Compare entry then choose Configure to open the Bom Compare version of the Report Manager dialog. Configure the report as needed then click Export. You also can select the desired output container then generate the report.

A BOM Compare can be performed from a number of places, including an OutputJob.

BOM Compare detects differences (delta) between the component items in the current design against the chosen released revision, creating a report listing only the component items that are different. It compares all parameters, excluding only dynamic parameters such as price and stock levels.

You can configure the columns that are visible in the BOM Compare report in the Report Manager.

The BOM comparison opens in the Report Manager, configure the columns as required.