How to Generate BOM Files from Altium Designer: A Complete PCB Engineer’s Guide

After spending years working with Altium Designer on everything from simple breakout boards to complex multi-layer designs, I can tell you that generating a proper Bill of Materials is one of those tasks that seems straightforward until you’re staring at a rejected assembly quote because your BOM was missing critical information. A well-structured BOM file isn’t just paperwork; it’s the communication bridge between your design and the manufacturing floor.

In this guide, I’ll walk you through every method Altium Designer offers for BOM generation, from the quick Reports menu approach to the more sophisticated ActiveBOM workflow that can save you hours of procurement headaches down the line.

What Is a Bill of Materials in PCB Design?

A Bill of Materials is essentially your shopping list for building a PCB assembly. It contains every component needed to populate the board, along with critical details that procurement and assembly teams need to source and place parts correctly.

Essential BOM Data Fields

Every manufacturing-ready BOM should include these core pieces of information:

Field	Description	Example
Designator	Unique reference ID on schematic/PCB	R1, C5, U3
Quantity	Number of identical components	4
Description/Comment	Component value or function	10µF 16V Ceramic Cap
Footprint	Physical package type	0805, SOIC-8, QFP-48
Manufacturer	Component maker	Texas Instruments
Manufacturer Part Number (MPN)	Exact part identifier	LM7805CT
Supplier Part Number (SPN)	Distributor’s catalog number	296-1465-5-ND

Missing any of these fields can cause delays, incorrect part orders, or assembly failures. I’ve seen projects slip by weeks because a BOM listed “10K resistor 0603” without specifying the tolerance, and the assembler had to stop production to ask which exact part to use.

Two Primary Methods for BOM Generation in Altium

Altium Designer provides two distinct approaches to creating BOMs, and understanding when to use each will make your workflow more efficient.

Method 1: Report Manager (Quick BOM Generation)

The Report Manager is the traditional approach, ideal for quick exports when you need a BOM right now and your component library already contains good parametric data.

Method 2: ActiveBOM Document

ActiveBOM is Altium’s modern BOM management system that treats the BOM as a living document throughout your design process. It connects to supplier databases in real-time, validates part availability, and catches sourcing problems before they become manufacturing delays.

For production designs, I strongly recommend using ActiveBOM. The upfront investment pays off when you’re not scrambling to find alternative parts at 2 AM before a deadline.

How to Generate a BOM Using the Report Manager

Let’s start with the faster method. This works well for quick prototypes or when you’re confident your library data is complete.

Step 1: Open the Report Manager Dialog

With your schematic project open in Altium Designer, navigate to the Reports menu and select Bill of Materials. This opens the Report Manager dialog, which displays all components found in your project.

The dialog is divided into two main sections: column configuration on the left and the actual BOM data grid on the right.

Step 2: Configure Visible Columns

By default, Altium shows basic component information. You’ll likely want to add more columns to make your BOM manufacturing-ready.

In the left panel, you’ll see a list of available parameters. Check the boxes for the columns you want to include:

Recommended Columns	Why Include It
Designator	Assembly reference
Comment	Component value
Description	Detailed part info
Footprint	Package verification
Quantity	Order quantities
Manufacturer 1	Primary source
Manufacturer Part Number 1	Exact part ordering
Supplier 1	Procurement source
Supplier Part Number 1	Order catalog number

Step 3: Choose Your Export Format

In the Export Options section of the Report Manager, select your desired output format from the File Format dropdown. Altium supports several options:

Format	Best Use Case
CSV (.csv)	Universal compatibility, easy spreadsheet import
Microsoft Excel (.xls, .xlsx)	Formatted reports with templates
PDF	Formal documentation packages
XML Spreadsheet (.xml)	Database integration
HTML	Web viewing
Text (.txt)	Simple text-based systems

For most manufacturing handoffs, I recommend Excel format with a custom template, or CSV for maximum compatibility with assembly house systems.

Step 4: Apply an Excel Template (Optional)

If you’re exporting to Excel format, you can apply a template to control the appearance and layout of your BOM. Altium includes several default templates in the Templates folder of your installation directory.

To use a template, enable the Template option in the Excel Options region and either select from the dropdown or browse to your custom template file.

Step 5: Export the BOM

Click the Export button, choose a filename and location, and save your BOM. If you’ve enabled Open Exported, Altium will automatically open the file in the appropriate application.

How to Generate a BOM Using ActiveBOM

ActiveBOM represents Altium’s recommended approach for serious production work. It provides real-time supply chain visibility and catches problems early in the design cycle.

Step 1: Create an ActiveBOM Document

Right-click on your project entry in the Projects panel and select Add New to Project followed by ActiveBOM. A new BomDoc will open showing all components currently placed in your schematic.

The ActiveBOM document automatically populates with every component from your design, organized by designator or other grouping parameters you specify.

Step 2: Review Component Solutions

This is where ActiveBOM really shines. For each component in your design, ActiveBOM searches the Altium Parts Provider database (powered by Octopart) to find matching manufacturer parts and available suppliers.

Each component row shows:

Status Icon	Meaning
Green (Clear)	Component has valid solutions with good availability
Yellow (Warning)	Solutions exist but minor issues flagged
Orange (Error)	Problems like NRND lifecycle status
Red (Fatal Error)	No solutions found or obsolete parts

Step 3: Configure BOM Columns

Open the Properties panel (View menu if not visible) and navigate to the Columns tab. Here you can enable or disable specific data columns and arrange their order.

For manufacturing BOMs, I typically enable:

Component Data: Designator, Comment, Description, Footprint, Quantity
Manufacturer Data: Manufacturer 1, Manufacturer Part Number 1
Supplier Data: Supplier 1, Supplier Part Number 1, Unit Price 1, Stock 1

Step 4: Set Component Grouping

In the Properties panel under BOM Items, configure how components are grouped. Options include:

Flat View: Every component instance on its own row
Base View: Components grouped by unique part, with all designators listed
Consolidated View: For projects with variants, shows all variants together

Most assembly houses prefer Base View, where identical components are grouped on single lines with combined quantities.

Step 5: Add Line Numbers

Click the Set Line Numbers button at the top of the ActiveBOM document to automatically assign sequential line numbers to each BOM entry. Many assemblers require line numbers for tracking during the manufacturing process.

Step 6: Export the Final BOM

Once your ActiveBOM is configured, generate the output file through Reports followed by Bill of Materials. The Report Manager dialog will appear with your ActiveBOM as the data source.

Select your format, apply any templates, and export.

Using Output Job Files for Repeatable BOM Generation

For production projects, creating an Output Job file lets you save your BOM configuration and regenerate identical outputs every time without reconfiguring settings.

Creating a BOM Output Job

Right-click your project in the Projects panel and select Add New to Project followed by Output Job File. A new OutJob editor opens with categories for different output types.

Under Report Outputs, click Add New Report Output and select Bill of Materials. Set the Data Source to either your project or your ActiveBOM document.

Configuring the Output

Double-click the BOM entry to open the Report Manager and configure columns, format, and template as described earlier. These settings are saved within the OutJob file.

Linking to Output Containers

Output Jobs use containers to define where generated files go. You can link your BOM output to:

Container Type	Purpose
File Generation	Saves to disk location
PDF	Creates PDF document
Print Job	Sends to printer

Right-click on an output container and select Generated Files Setup or PDF Setup to configure output paths and naming conventions.

Generating Outputs

Once configured, you can generate your BOM anytime by right-clicking the container and selecting Generate Content. The same configuration produces identical results every time, which is essential for revision control and reproducibility.

Best Practices for Manufacturing-Ready BOMs

After years of back-and-forth with assembly houses, these practices have become non-negotiable in my workflow.

Always Include Manufacturer Part Numbers

Generic descriptions like “100nF capacitor” aren’t sufficient for production. Assemblers need exact MPNs to source the correct parts. Even for passives, specify complete part numbers.

Add Alternative Parts When Possible

Supply chain disruptions happen constantly. Using ActiveBOM, you can define multiple solutions (alternate parts) for each component. When your primary part is unavailable, the assembler has pre-approved alternatives ready.

Verify Lifecycle Status

ActiveBOM automatically flags components with concerning lifecycle statuses:

Status	Risk Level	Action
Active	Low	Safe to use
NRND (Not Recommended for New Designs)	Medium	Consider alternatives
Last Time Buy	High	Source immediately or replace
Obsolete	Critical	Must replace
EOL (End of Life)	Critical	Must replace

Catching an obsolete part during design is vastly preferable to discovering it during production.

Include Footprint Information

Always include footprint data in your BOM. This gives the assembler a cross-check that the parts received will actually fit the pads on your PCB. Mismatches between BOM part numbers and PCB footprints are surprisingly common errors.

Mark DNP Components Clearly

Components that shouldn’t be populated (DNP or Do Not Place) need clear marking. In Altium, set the component type to Standard (No BOM) in schematic properties, or use the Variants feature to define which parts are populated in each product version.

Common BOM Generation Problems and Solutions

Even experienced designers run into these issues occasionally.

Missing Components in BOM

Problem: Some parts from your schematic don’t appear in the generated BOM.

Solutions:

• Verify the project is compiled (Project menu then Compile)
• Check that components aren’t set to Standard (No BOM) type
• Ensure hierarchical sheets are properly connected to the project

Wrong Quantities

Problem: BOM quantities don’t match actual component count.

Solutions:

• Recompile the project to refresh component counts
• Check for duplicated designators across schematic sheets
• Verify that component grouping settings are correct

Missing Manufacturer Data

Problem: MPN and manufacturer columns are empty.

Solutions:

• Add manufacturer parameters to library components
• Use ActiveBOM to manually add part choices
• Link components to the Altium Parts Provider database

Solution Not Recognized Error

Problem: ActiveBOM shows “Solution is not recognized” for parts that clearly exist.

Explanation: Altium’s Octopart database can’t guarantee 100% coverage of all parts. This warning indicates the system can’t verify real-time availability status.

Solution: Verify part availability directly on distributor websites and consider adding the information manually to your BOM.

Useful Resources for Altium BOM Management

Here are the key resources for deepening your BOM skills:

Official Altium Documentation:

• BOM Management with ActiveBOM: altium.com/documentation/altium-designer/activebom
• Report Manager Documentation: altium.com/documentation/altium-designer/bom-configuration-report-manager
• Output Jobs Guide: altium.com/documentation/altium-designer/preparing-for-manufacture/output-jobs

BOM Templates:

• Default templates location: [Altium Install Directory]\Templates
• Custom templates can be created in Excel and referenced in Report Manager

Supply Chain Data:

• Octopart: octopart.com (Powers Altium Parts Provider)
• Component data aggregation used by ActiveBOM

Altium Training:

• Altium Academy: altium.com/academy
• Video tutorials covering BOM workflow

FAQs About Generating BOMs in Altium Designer

Can I include pick and place data in my BOM?

Yes. In the Report Manager dialog, enable the Include Parameters From PCB option. This adds columns for X/Y coordinates, rotation, and layer information. However, most assembly houses prefer a separate centroid file (Generates via File then Assembly Outputs then Generates pick and place files), so check with your manufacturer about their preferred format.

How do I exclude specific components from the BOM?

There are two approaches. First, you can set the component’s Type property to Standard (No BOM) in the schematic symbol properties. Second, for production variants where components are conditionally populated, use Altium’s Variants feature to define which parts appear in each variant’s BOM.

What’s the difference between generating a BOM from the project versus from ActiveBOM?

When you generate from [Project], the Report Manager extracts component data directly from schematic documents. When you generate from [ActiveBOM Document], it uses the curated, supply-chain-aware data you’ve configured in the BomDoc, including manually added solutions, supplier preferences, and verified part choices. The ActiveBOM approach gives you more control and better data quality.

Can I add non-PCB items like mounting hardware to my BOM?

Yes, ActiveBOM supports adding custom BOM items that don’t exist as placed components. In the ActiveBOM document, use the Add Item button to add entries for things like bare PCBs, screws, standoffs, enclosures, labels, or conformal coating. These items appear in the final BOM alongside your electronic components.

How do I update supplier pricing data in my BOM?

In the ActiveBOM document, pricing and availability data updates automatically when connected to the internet through Altium Parts Provider. You can also manually refresh by right-clicking and selecting Refresh Selected. For cached data when working offline, use the Cached option instead of Real-time in the Report Manager settings.

Conclusion

Generating a quality BOM from Altium Designer isn’t complicated once you understand the tools available. For quick prototypes, the Report Manager gives you fast results. For production designs where supply chain visibility and part availability matter, ActiveBOM provides the control and real-time data you need to avoid manufacturing delays.

The key is building good habits early: populate your library components with complete manufacturer data, use ActiveBOM to validate sourcing before finalizing designs, and create Output Job files so your BOM generation is repeatable and consistent across revisions.

Your assembler will thank you for a complete, accurate BOM. More importantly, your project will ship on time.