Sourcing, Lifecycle and Bill of Materials

• A BOM is a contract with your future self and your assemblerIt must uniquely identify what to buy. That means manufacturer name plus manufacturer part number, not 'MOSFET 30 V'. Ambiguity in a BOM becomes a wrong part on a board, and the cost of finding that is enormous compared to the cost of writing it down properly.
• MPN, distributor part number and the differenceThe manufacturer part number identifies the component. A distributor part number identifies a specific packaging and stocking arrangement of it. Include the MPN always; the distributor number is convenient but must never be the only identifier, because distributors change and disappear.
• Lifecycle status drives design riskActive parts are safe. NRND means the manufacturer will not support new designs and end-of-life is coming. Last Time Buy and Obsolete mean you are designing in a future redesign. Check status at design time and again before every production run.
• Availability, lead time and MOQA perfect part with a 52-week lead time is not available. Check stock across at least two distributors, note the lead time, and note the minimum order quantity and packaging multiple. A part sold only in 3000-piece reels is a problem for a 10-board prototype run.
• Alternates and do-not-substituteFor every line, decide whether a substitution is acceptable. Generic passives usually are, provided the specification fields are met. Anything whose behaviour is defined by more than its value — regulators, references, crystals, connectors, anything with a footprint that must match — should be marked do-not-substitute, and the reason recorded.
• Second sourcingFor critical lines, identify a second manufacturer's part that is footprint and function compatible, and verify the compatibility yourself rather than trusting a cross-reference tool. This is the difference between a supply shock costing you a week and costing you a redesign.
• The BOM lives in the schematicManufacturer, MPN, package and any do-not-substitute note should be fields on the schematic symbol, so the BOM is generated rather than maintained separately. A hand-maintained BOM diverges from the schematic within days.
• Do-not-populate and variantsDNP lines are part of the design, not omissions: they document deliberate options, jumpers and test points. A BOM must state them explicitly, because an assembler seeing a footprint with nothing assigned will ask, or worse, guess.

ProblemYou have a 40-component schematic. Convert it into a BOM an assembly house can quote from without asking you a single question.

1. 1
   Group by identical part: your 12 100 nF capacitors become one line with 12 references, not 12 lines. Grouping is how quantity discounts and reel counts are computed.
2. 2
   For every line, populate: quantity, reference designators (C1, C4, C7...), value, package/footprint, manufacturer, MPN, description, and lifecycle status.
3. 3
   Passives: add the full specification to the description field, e.g. '100 nF, 50 V, X7R, 0603, +/-10%'. Mark substitution as allowed provided the specification is met.
4. 4
   Actives and anything with a specific footprint: mark do-not-substitute and record why in a notes column, e.g. 'pin 1 orientation differs on alternate' or 'stability requires specified Cout ESR'.
5. 5
   Connectors: these are the most-substituted and most-wrongly-substituted lines on any BOM. Always do-not-substitute, always include the mating part number in the notes.
6. 6
   Check stock: for each active line, record stock quantity and lead time from two distributors, with the date checked. A BOM without a date is a BOM of unknown validity.
7. 7
   Add a second source for every do-not-substitute line where one exists, and verify pinout and footprint compatibility from both datasheets, not from a cross-reference database.
8. 8
   Add DNP lines with a note explaining the option each one represents.
9. 9
   Add a header block: board name, revision, date, author, and the schematic revision this BOM was generated from. A BOM that does not name its schematic revision is dangerous.
10. 10
    Generate it from KiCad rather than typing it, so it regenerates when the schematic changes.

AnswerA grouped, fully-specified, dated BOM generated from schematic fields, with lifecycle and stock checked per active line, explicit substitution policy per line, second sources for critical parts, DNP lines documented, and a header tying it to a specific schematic revision.

Tool: KiCad BOM generation with custom fields

• Open a KiCad schematic. Open the Symbol Fields Table (Tools > Edit Symbol Fields, or the equivalent in your version).
• Add custom columns: Manufacturer, MPN, Package, Lifecycle, Substitution, Notes.
• Fill them in for every symbol. Use the table view to fill many rows at once — this is far faster than editing symbols individually.
• Enable 'Group symbols' in the table so identical parts collapse into single rows and you can see your part-number count.
• Use the DNP checkbox on symbols that are deliberately unpopulated, and add the reason in Notes.
• Export the BOM: File > Export > Bill of Materials (or Tools > Generate BOM depending on version). Choose or configure a format that includes your custom fields.
• Open the exported CSV. Verify: references are grouped, quantities are right, every active line has an MPN, and the DNP lines are marked.
• Deliberately change one symbol's value in the schematic and regenerate. Confirm the BOM updates. This proves the BOM is generated, not maintained.
• Commit both the schematic and the generated BOM to version control. Diff the BOM between two commits to see exactly what changed between revisions.

• KiCad documentation - BOM generationopen licencedoc~45 minSee the schematic editor manual's BOM section, and the symbol fields table. Free and open.
• Octopart / distributor parametric search and stock checkfreetool~30 minFree search across distributors for stock, price breaks and lifecycle. Proprietary, but there is no open equivalent with live inventory data.
• KiCad's KiBoM / kicad-jobset BOM toolingopen licencetool~60 minKiBot is an open-source automation tool that generates BOMs, gerbers, assembly drawings and more from KiCad files in CI. Worth adopting early.
• Assembly house documentation requirements (e.g. a PCBA vendor's guide)freereference~30 minRead what a real assembler actually requires: BOM format, centroid file format, and their part-matching rules. Designing to a real recipient's requirements is the point.

Take a real schematic — your own, or an open-hardware design you can download — and produce a complete, dated, buildable BOM package plus a supply-risk assessment.

Deliverables

• A generated (not hand-typed) BOM from KiCad, grouped, with columns for quantity, references, value, footprint, manufacturer, MPN, description with full specification, lifecycle status, substitution policy, and notes.
• Evidence that the BOM is generated: two exports from two schematic revisions with a diff showing exactly what changed.
• A stock and lead-time check for every active component from at least two distributors, with quantities, price at 10 and 100 units, and the date checked.
• A supply-risk assessment identifying the three highest-risk lines with a stated reason (single source, long lead time, NRND, high MOQ, sole-source connector) and a mitigation for each.
• A verified second source for at least two critical lines, with a side-by-side comparison of the parameters and footprints that had to match, citing both datasheets.
• A do-not-populate section listing every DNP with the design option it represents.
• A total build cost at 10 units and at 100 units, with the components contributing the top 20% of cost identified.

Acceptance criteria — how you know it is good enough

• Every line has a manufacturer and a manufacturer part number.
• The BOM was generated from the schematic and this is demonstrated, not asserted.
• Lifecycle status is present and dated for every active part.
• Second-source compatibility is verified against datasheets, not taken from a cross-reference tool.
• Substitution policy is explicit for every line, and connectors are do-not-substitute.
• The header ties the BOM to a specific schematic revision and date.

If you want to push further

• Set up KiBot in a CI pipeline so the BOM, gerbers and assembly drawings regenerate automatically on every commit.
• Re-cost the design substituting your top three cost drivers with functionally equivalent alternatives and quantify the saving against the engineering time to qualify them.

• Every part in my designs carries a manufacturer and MPN in the schematic itself.
• My BOMs are generated from the schematic and cannot drift from it.
• I check lifecycle status and stock before committing a part, and I date the check.
• I mark substitution policy per line and never allow connectors to be substituted freely.
• I can verify a second source's compatibility from datasheets.
• I document DNP lines as design options rather than leaving them blank.