Creating the ActiveBOM Document in Altium NEXUS

Parent page: BOM Management with ActiveBOM

Creating the BOM Document

ActiveBOM's working BOM document is referred to as a BomDoc. Add a new BomDoc to the project via the File » New sub-menu, or right-click on the project in the Projects panel. When there is at least one component in the project, a new BomDoc can be created by clicking the + Create control next to the ActiveBOM entry within the project structure in the Projects panel. Note that each PCB project can only include one BomDoc.

When you add a new BomDoc to your project, the schematic is automatically compiled and all of the existing components are listed in the BomDoc. For Workspace Library components that include Part Choices, Solutions will be detailed in the lower region of the interface, as explained in the Understanding the Solution section below.

As additional components are placed on the schematic they are automatically added into the BomDoc. Additional BOM Items and additional parameters can also be manually added directly in ActiveBOM, via the Add new button, located above the component list. Refer to the Custom BOM Items and Columns section to learn more.

The BOM Items List

The upper region of the BomDoc is a tabular list of all of the components detected in the PCB design project, as well as additional BOM Items you have added directly into the BomDoc. This region is referred to as the BOM Items list.

The components, or BOM Items list, displayed in the Base view.

There are 3 view modes available to display the BOM Items. Select the required mode using the buttons located above the list:

 Flat view - a row for every component.

 Base view - a row for each unique component in the project, the Designator column lists the designators of all components of this type. Multiple presentation options are available for grouped designators. Select the required Designator Grouping mode in the Properties panel.

 Consolidated view - used when the project includes variants, to display a consolidated BOM for all variants.

The Column Groups

The ActiveBOM components list has distinct groups of columns that present in each view mode, the image above shows the Base view.

The BOM Items grid is clustered into the following major groups:

1. Item Details (orange highlight in the image) - these columns display parametric component details, such as the Designator, Description, Library Reference, and other component parameters.
2. Solutions (cyan highlight in the image) - the highest-ranked manufacturer + supplier(s) from the Supply Chain. The number of solutions (manufacturer parts), and the number of suppliers of each solution, are configured in the ActiveBOM Properties panel - these are indicated by a  solid, colored banner in the supplier tile. Ranking is automatic, and can also be manually defined, as discussed in the Understanding the Solution section below.
3. BOM Status (green highlight in the image) - an indication of the current risk associated with each component. Hover over an icon for a description, or alternatively, enable the detailed BOM Status column in the Properties panel to display the description.
4. Variant Details - in Consolidated View, an additional Group, titled Variants, is added just before the BOM Status column. This group includes a column for the base design, and one for each variant, displaying the quantity (per unit) of each component. Refer to the Working with Variants section for more information.

Custom BOM Items and Columns

BOM management for a PCB design project requires the management of components and BOM Items beyond those placed in the schematic and PCB. There are many cases when custom BOM Items or parameters will be used in the PCB design project. For these situations, ActiveBOM supports adding additional BOM Items and columns (parameters), which can then be included in the generated BOM:

• Custom row -  an easy way to add a custom BOM Item that needs to be accounted for in the design (bare board, glue, etc). All fields in a custom row are user-defined. Custom rows are not managed by ActiveBOM, for example, if the quantity is set to 3, there will not be 3 separate items displayed in Flat view. Supply chain searching is also not supported for custom rows.
• Custom column - additional BOM column, managed in ActiveBOM, that can contain any user-defined text.
• Custom Item - an additional BOM Item, this is typically for those items that will be needed but are as yet not fully known or do not yet exist in the library. This allows these items to have their cost included in the overall board cost estimation.
• Managed Component - an additional BOM Item, that is managed manually in the BOM document. The Component Search dialog will open, listing the components in the currently connected Workspace. The chosen additional BOM Item can also be changed at any time via the right-click Operations sub-menu.

Data Sources

The default data sources available in ActiveBOM are the schematic component parameters ( ), the Workspace component parameters for Workspace content ( ), and data provided by ActiveBOM ( ). From these sources, ActiveBOM generates the main project BOM Item grid. Data sources are enabled and their display controlled in the Columns tab of the ActiveBOM Properties panel.

By enabling the relevant Sources button (above the Columns list), the BOM can also include information taken from the following additional data sources:

The PCB - enable these to include PCB location/rotation/side of board data in the available Columns, for each of the components.

Database - to load additional component parameters from an external database (via *.DbLib, *.SVNDbLib, or *.DbLink).

 Altium Cloud Services - enable this to access a broad range of additional component data, for those BOM Items that have been identified by the Altium Parts Provider and show a supply chain solution.

 Document Parameters - enable this to include all detected schematic document parameters, across all schematics in the PCB project in the available Columns.

The source of each parameter is indicated by the icon in the list of columns.

Line Number Column

For PCB designs with assembly drawings, or for BOM data exchange between design engineers, cost engineers or purchasing specialists, the BOM line number (BOM Item position No) is a simple method used to individually distinguish BOM lines, which can then be used to explicitly identify or find the corresponding callout, component and depiction in the design.

As the project BOM data source, ActiveBOM supports user-defined Line #’s for the project BOM and has both manual and automatic Line # (BOM Item position No) management features.

• To automatically set the position number for the all project BOM Items (components), click the Set Line # button. Line numbers are displayed in the Line # column, in the Item Details group of columns. Click the dropdown icon on the right of the button to open the Line # Options dialog, where the start and increment values can be defined.
• To manually change Line #'s, switch to Base view mode then select the required cell(s) in the Line # column and:
  • Press Delete on the keyboard to clear the cells, then
  • manually type in new values, or
  • paste a range of values from the Windows clipboard.
• To renumber or continue numbering from a custom added number click on the required item Line # cell, then click the Set Line # button. The Line Numbering dialog will open, where you can Continue numbering or Renumber all. The base and increment values last defined in the Line # Options dialog are used to calculate the numbers added, if required you can enter a seed value in the selected Line # cell to define the start number.

Configuring and Saving the Display of the BOM Items Grid

Like any good spreadsheet application, the BOM Items grid can be configured to suit your requirements. As well as the traditional column ordering and sorting features, the current configuration can be saved as a BOM Set.

Working with BOM Sets

Any number of BOM Item grid configurations can be saved - each of these is referred to as a BOM Set. After configuring the grid to your requirements, click the Add button in the BOM Sets region of the ActiveBOM Properties panel to add a BOM Set to the list.

Click the eye icon to enable a BOM Set.

BOM Sets are configured in the ActiveBOM Properties panel.

Replacing a Component

It's not uncommon to identify an issue with a component when the BomDoc is being checked and made ready for ordering the parts. For example, the designer may have forgotten to finalize the selection of a component, or a component has gone EOL and the designer wants to explore the price and availability of potential replacements. Previously the only way to resolve this was to return to the schematic and edit the component, select a suitable part, then refresh the BomDoc.

Alternatively, you can change a component in the BomDoc, and then pushing that change back to the schematic via an Engineering Change Order. Right-click on the selected component(s) and select the Operations » Change <ComponentName> command. The Replace Component dialog will open, where the replacement component can be searched for.

When the Replace Component OK button is clicked the Engineering Change Order dialog will open, detailing the changes needed to synchronize the schematic with the BomDoc.

Working with Variants

ActiveBOM supports PCB projects that include Design Variants. The Design Variants feature allows a single base PCB design to be created, which is then populated (loaded) in different ways. Each different loading of the assembled board is called a design variant.

Working with Design Variants:

• Design variants are configured in the Variant Management dialog (Project » Variants).
• To examine a variant, double-click on its name in the project's Variants folder in the Projects panel, as shown in the image below.

ActiveBOM supports variants in the following ways:

• Display the BOM for a specific variant in Base view mode or Flat view mode
• Option to include the Not Fitted items in the BOM Items list
• Display a consolidated list of all parts used in all variants, in Consolidated view mode
• Define manual solutions for both base components and varied components

Variants in Base View Mode

For the selected variant, enable the Show Not Fitted option in the Properties panel to include these parts in the BOM Items grid. When this option is enabled, the Fitted column is automatically displayed in the Item Details.

In Base view mode the Fitted column will display either Fitted or Not Fitted. If a part is varied (an alternate part was chosen in this variant), the details of the alternate part are automatically displayed for that BOM Item.

Note that the current variant is displayed in the ActiveBOM status line.

Variants in Consolidated View Mode

The Consolidated view mode displays all components used in all variants. The Consolidated view offers the following features:

• If a component is varied, there will be a BOM Item for each alternate component that is used, with each of these BOM Items having the same designator. For example, in the image below, components DS1 and DS2 are each list twice, as the BGA variant uses a different colored LED from the TSOP variant. Component R1 appears three times because both the BGA and TSOP variants use a different resistor than the original in the base design.
• In Consolidated view mode, when the Show Not Fitted option is enabled the Fitted column will display Fitted or Varied. Because the Consolidated view shows all components used in all variants, every component displayed is fitted in either the base or a variant.
• For each variant, there is a <VariantName> - Qty column (indicating how many of this component are used in this variant) and a <VariantName> - Price column, which is the unit price times the value in the quantity column.
• Because some designers create build documentation off the base design as well as the variants, there is also a Quantity column, reflecting the number of instances of this component used in a build of the base design. Hide this column if you do not generate build documentation off the base design.
• The grid in Consolidated view mode uses color to indicate a cell whose value is different from that cell's value in the base design, as shown below.

Color in a cell indicates that the value in this cell is different from the value for that cell in the base design.

To learn more about variants, refer to the Design Variants page.

Working Between the BomDoc, the Schematic and the PCB

There are two features available to help you work between the BomDoc, the schematic and the PCB design: Cross Select and Cross Probe. The behavior of these features is configured in the System - Navigation page of the Preferences dialog.

Both of these features can be used to locate the same component in other documents. The difference between Cross Select and Cross Probe is that Cross Select Mode selects the component in the target document but does not actively present that document, whereas Cross Probe actively presents the target document, and can also switch and make the target document's editor the active editor.

You can Cross Select or Cross Probe from the BomDoc to the schematic and PCB, you can not Cross Select or Cross Probe from the schematic or PCB, to the BomDoc.

Cross Select Mode

Cross Select Mode must be enabled in each editor in which you wish to use it. Select the Tools » Cross Select Mode command (Shift+Ctrl+X). When Cross Select Mode is enabled the menu icon will be highlighted with an outline .

Cross Select Mode requires the target document to be open. When you select a component in the BOM Items list of the BomDoc, that component will be selected and centered in the target schematic and PCB documents (if Zooming is enabled in the Cross Select Mode options in the Preferences dialog). Note that the target document will not present as the active document.

If the BomDoc is in Base view mode, then all instances of that part are selected on the schematic and PCB, as shown in the image below.

Use the Cross Select feature to locate and select the component chosen in the BOM Item list, in the schematic and on the PCB.

Cross Probing

Where Cross Select is simply a mode, which when enabled, displays the result each time you click in the BOM Items list, Cross Probe is a deliberate action.

Right-click on a BOM Item and select Cross Probe from the context menu to cross probe to that component on the schematic, the PCB component will also be cross probed to if the board file is open.

A key feature of Cross Probe is the ability to switch to the target document's editor. To Cross Probe and switch editors, hold the Ctrl key as you select the Cross Probe command.

Right-click to access the Cross Probe command, there will be an entry for the designator of each component present in that BOM Item.

Properties Panel

When the active document is a BOM document (*.BomDoc), the Properties panel presents the Document Options.

The following collapsible sections contain information about the options and controls available: