Setting the New Standard in Electronics Design.

Efficiency. Collaboration. Accuracy.

Switch and Get the Power to Design Without Limits

Get 50% off when you switch to Altium Designer before April 26, 2024

Art of Schematic / Using the ActiveBOM Completed Sign In To Save Your Progress
Click if you find this content useful

Art of Schematic

Using the ActiveBOM

A BOM (bill of materials) is a document that needs to be obtained during the PCB design process. This document contains a list of all the components with their designators, part numbers, values, and other parameters. If the schematic is ready, we will not make any more changes; we can now create this document with the ActiveBOM editor. This powerful tool combines comprehensive BOM management with Altium Designer's part information aggregation technologies, helping you manage the component selection challenge.

Ensure that the project is active so that the ActiveBOM document will be attached to the correct project. To activate the project, open one of the project's schematic sheets. On the list of projects, the active project is highlighted.
Project Kame_FMU.PrjPCB is activated.
Fig. 1 - Project Kame_FMU.PrjPCB is activated
Add a new ActiveBOM document to the project. To do this, select File > New > ActiveBOM. A new document will appear in the Kame_FMU project tree, and a new tab will open with a list of all components.
Creating a new ActiveBOM document.
Fig. 2 - Creating a new ActiveBOM document


The ActiveBOM editor tab.
Fig. 3 - The ActiveBOM editor 
The manufacturer's solution will appear for all components in the project. For each component, you will see the proposed part number, manufacturer, current component lifecycle stage, unit price, and total price. Powered by Octopart and Ciiva, the ActiveBOM engine automatically compares prices for all presented components from all selected suppliers and chooses the best solution for you. You can select your favorite suppliers in the Supply Chain region of the Properties panel by clicking the Edit button associated with the Favorite Suppliers List. In the Project Part Providers Preferences dialog box, you can uncheck suppliers you don't need and focus only on available providers. You can also set suppliers' priority. After making any necessary changes, click OK to save the changes.
Editing the Part Suppliers List.
Fig. 4 - Editing the part suppliers list
Click on a component in the ActiveBOM to display all the suggestions for that component. Selected information about the availability and cost of the component is displayed at the bottom of the window, allowing you to compare all possible solutions. Click the desired component/supplier.

Tip: For grouped designators, use the Designator Grouping drop-down in the BOM Items region of the Properties panel to choose the presentation.

Part Solutions and Suppliers Suggestions for the Selected Connector.
Fig. 5 - Part solutions and supplier suggestions for the selected resistor
The ActiveBOM includes a set of BOM rules that must be followed in order to obtain all components without any issues. The rules automatically check each component. The status of each check is displayed as follows:

Clear icon – Clear: There is a solution for the component; all components are available from the supplier.

Warning icon– Warning: There is a solution for the component, but there are some minor warnings.

Error icon – Error: There is a solution for the component, but there are specific problems with this component in the design, such as an outdated component revision in your schematic, NRND (Not Recommended for New Design), etc.

Fatal Error icon – Fatal Error: No solution for this component needs rectifying. Reasons for this error include restricted usage of a component with an obsolete lifecycle status, components not found from the suppliers, and suppliers' data not being updated for a while.

Tip: You can hover the mouse over the error to view the entire error text.

You can see errors and filter them based on their type in the BOM Checks region of the Properties panel. At this stage, we have many warnings with the Violation Type "No MPN (Manufacturer Part Number) ranked" because we still need to add our rating for the suggested solutions. This warning will be fixed later in this section.
The BOM Checks Region in the Properties panel is Used for BOM Error Checks
Fig. 6 - BOM Checks region of the Properties panel

Tip: To sort the BOM Checks region, click on the column heading by which you want the region sorted. To filter the region and show only violations of a certain type(s), click the filter icon of the desired violation.

Confirm the suggested manufacturer solutions and, if necessary, replace components from our list. To do this, it is easier to sort the list into groups. Let's group our components based on their designator to assign the same solution to all the same components automatically. Many capacitors, resistors, and resistor assemblies will be combined into groups for our purposes. To do this, click Group at the top left of the BomDoc, then enable Designator in the drop-down menu. All components are now grouped, and each line is a list of components with the same part number.
Component Grouping Based on Their Designators
Fig. 7 - Component grouping based on their designators

Let's take a look at the largest group of capacitors. Expand this section and then click on a line to see the suggested part solution. We can see a warning that we have no MPN ranking. A new BOM item's default state is that the suppliers are ranked automatically. Using a five-star rating scale, you can set your personal preferences when selecting components. The ActiveBOM engine will list components with the highest rating. Let's define the rank of this group. Take a look at the Manufacturer Part region. You may notice that each component of each supplier's name is highlighted. Green indicates the optimal solution in terms of price, supplier availability, lifecycle stage, and other parameters. Orange denotes an acceptable part and supplier solution, although it may be more expensive or only small quantities are at the supplier's disposal. Red indicates a risky solution; components could be at the end of the lifecycle, or insufficient quantities are in stock. Also, the current component lifecycle stage is displayed in the available solution list. Choose a solution highlighted in green; rate it five stars by clicking on the rightmost star. The warning for this group will disappear, and the status will turn green.

Component C0402C104K8RACTU is Ranked Five Stars as a Solution
Fig. 8 - Green status of components with five-star ratings

Tip: If desired, you can change the rank or remove it by clicking the trash can icon associated with the rating.

You can automatically assign a five-star rating to the most appropriate component in the ActiveBOM version by expanding the next group, right-clicking the group’s name, and selecting Set Ranks Automatically. The maximum rating for the most suitable and profitable component is automatically set.

Automatically Assigned Rank for the Most Suitable Solution for this Component
Fig. 9 - Set ranks automatically for the most suitable solution for this component
Now let's set the ranks automatically for all the remaining components with this warning. Remove the designator grouping by clicking Group at the top-left of the BomDoc and then disable the Designator checkbox. Click the filter icon associated with the No MPN ranked violation type in the BOM Checks region of the Properties panel to show only components with this warning.
Enable Filtering for Components with the No MPN ranked violation
Fig. 10 - Enable filtering for components with No MPN ranked
Hold the Shift button, select all components in the BOM list, right-click on one of the selected parts, and then select Set Ranks Automatically from the context menu. The warning is now fixed for all components.
Components with Current Warnings
Fig. 11 - Components with current warnings
There is a fatal error with CN1 and CN2. Hover the mouse over the error icon to see that the component revision is outdated and restricted for usage. Therefore, we must update this component on the schematic to the latest revision. We can quickly locate this component by right-clicking it and then choosing Cross Probe. We also need to select the schematic sheet(s) on which this component is placed. In our case, two components are placed on the same sheet. After selection, the schematic sheet will open, and you will see the violating component.
Cross Probe the Outdated Component
Fig. 12 - Cross probe the outdated component
You can update only the selected component by selecting Tools > Update Selected From Libraries. However, we recommend updating all components using the Item Manager dialog (Tools > Item Manager). Click the Lifecycle State column header to sort the list by that column. Components with Obsolete status should be at the top of the list. As you can see, there is an additional component in the Obsolete lifecycle state. This is why all components are updated - not only the selected component.
Update From Libraries Configuration
Fig. 13 - Update from libraries configuration
Select all Obsolete components. Right-click on one, then select Update to the latest revision.
Updating Components to the Latest Revision
Fig. 14 - Updating components to the latest revision
The New Settings region on the right side of the dialog is now completed for the selected components. We must apply the new settings by generating an engineering change order (ECO). Click the ECO button at the bottom of the dialog, then select Generate ECO. In the dialog that opens, validate and execute the changes, and be sure to set new parameters.
Generating an ECO for Obsolete Components
Fig. 15 - Generating an ECO for obsolete components
Open the BomDoc. Right-click and then select Refresh selected to update the part solutions.
Find the U12 component. Hover the mouse over the error icon. This component has No solutions, so let's add a solution manually.
Solution is Missing for U12 Component
Fig. 16 - Solution is missing for the U12 component
To do this, click the Add Solution button above the Manufacturer Part region and select Create/Edit Manufacturer Links. The Edit Manufacturer Links dialog box opens.

Tip: You can also open the Create Manual Solution dialog by right-clicking on a component in the BOM grid and selecting Add Solution > Create Manual Solution.

Create Manufacturer Links for the Capacitor Group with the NRFND Lifecycle Stage
Fig. 17 -
Create manufacturer links for the group with the NRND lifecycle stage


The Edit Manufacturer Links dialog
Fig. 18 - The Edit Manufacturer Links dialog
Click the Add button to select the component. The Add Part Choices dialog box allows you to select the desired part solution. This dialog is similar to the Manufacturer Part Search panel that can be used during schematic component placement. Part number STM32F427VIT6 of the U12 component has been entered automatically as a search request, and there is an available solution. Select the available solution, then click OK to apply the changes.
Part Solution Selection
Fig. 19 - Selecting the part solution 

Tip: Click on nn SPNs in the selected solution to see its availability, price, etc.

After selecting the solution and closing the Add Part Choices dialog box, you'll see that the selected solution is now displayed in the Edit Manufacturer Links dialog. Click OK to proceed with the selection. The selected part choice is now defined for U12 as shown by its state. Remember to rate the solution!
Selected Solution is Shown in the Edit Manufacturer Links Dialog
Fig. 20 - Selected solution is displayed in the Edit Manufacturer Links dialog


Updated Manufacturer Part Number for U12
Fig. 21 - Updated manufacturer part number for U12
We also have two mounting holes defined as components in our BOM. Select PTH1 and PTH2 in the BOM grid, right-click, and then select Add Solution > Create Manual Solution.
Creating a Manual Solution
Fig. 22 - Creating a manual solution
In the Create Manual Solution dialog that opens, specify the solution parameters by entering them as shown below, then click OK to save the solution settings.
Configuring the Manual Solution
Fig. 23 - Configuring the manual solution

That's it - our document is ready and Altium Designer is up-to-date using modern, accurate, and convenient process. It will be generated to a separate file (for example, .xlsx) using an OutJob, which is described in a separate chapter.

Good job! Article is now completed!
Sign In To Save Your Progress

Read Again

Was this article useful?
Yes No
Thank you Glad to hear it