PCB & manufacturing
PCB Manufacturing Package Checklist: What Files Should You Send?
The three groups of files a manufacturing package contains, the errors that cost money, what to ask your manufacturer, and a checklist to work through before you send.
Requirements vary. Every fabricator and every assembler has its own list, and some accept formats others reject. This is not what everyone demands — it is what is worth having ready and checked before you ask yours what they want.
What is a PCB manufacturing package?
A manufacturing package is the set of files that lets somebody else build your board without asking you questions. It splits into three groups: files that make the bare board, files that populate it, and files that say which version of the design all of this is.
Most problems come from the third group being missing.
Fabrication: what makes the bare board
| File | What it is | What to check |
|---|---|---|
| Gerbers | one file per layer — copper, soldermask, silkscreen, paste | every layer the stackup declares is present, and no extra ones |
| Drill files | Excellon, usually plated and non-plated separately | whether diameters are finished or tooling size — say which |
| Board outline | the mechanical profile | exactly one, closed, on one layer |
| Stackup | layer order, thicknesses, materials | copper layer count matches the Gerbers |
| Fabrication drawing | notes, finish, tolerances, hole table | states surface finish and final thickness |
| Impedance requirements | which traces are controlled, to what value | your fabricator will usually adjust the stackup to hit it — ask early |
The outline deserves its own sentence
More boards are delayed by an ambiguous outline than by anything else in this list. If the profile appears on two layers, or is drawn as four unconnected lines, the fabricator either guesses or stops and emails you. Both cost days.
One closed profile, on one clearly named layer, and mentioned in the drawing.
Assembly: what populates the board
| File | What it is | What to check |
|---|---|---|
| BOM | the parts list | manufacturer and MPN on every line; DNP lines present and marked |
| Pick-and-place / centroid | reference, X, Y, rotation, side | origin stated; DNP parts not included |
| Assembly drawing | what goes where, and in which orientation | shows polarity and pin 1 |
| Polarity information | diodes, electrolytics, connectors, ICs | on the silkscreen and on the drawing |
Fabricator and assembler are often different companies
This is worth saying plainly because it changes what you send. The fabricator needs the first table and nothing from the second. The assembler needs the second, plus the bare boards. If one company does both, they will still usually want the two sets separated.
Sending an assembler your stackup does no harm. Sending a fabricator your BOM does no harm either. But assuming one package covers both is how a board gets fabricated without anyone noticing that the BOM was never reviewed.
Control: which version is this?
The group that gets skipped, and the one that costs most later.
| Item | Why it matters |
|---|---|
| Board revision | which design this package describes |
| Release identifier | so two packages from the same month can be told apart |
| Date | ordering, when the identifier is ambiguous |
| Approved source | which design version it was generated from |
| Manufacturing notes | anything that does not fit in a file: acceptable alternates, acceptance criteria, special handling |
A package with no revision identity is a ZIP that somebody will have to reverse engineer in eighteen months. It costs nothing to add and it is the single highest-value item in this article.
The errors that actually cost money
1. Drill diameters with no statement of finished vs tooling. Holes come out the wrong size and connectors do not fit. Say which you exported.
2. An open or multi-layer outline. Covered above. Still the most common delay.
3. Extra layers. An internal notes layer exported as copper gets fabricated. Check the layer list against the stackup, every time.
4. DNP parts deleted from the BOM. The assembler sees an empty footprint, assumes a missing line, and populates it from a similar reel.
5. Centroid and Gerbers with different origins. Everything is placed offset. Check the assembler's preview before approving.
6. No revision identifier on the package. Two sends in one month and nobody knows which was built.
7. A ZIP with no manifest. The supplier will usually ask. The expensive case is when they do not.
What to ask your manufacturer
Do this once, write the answers down, and reuse them:
Gerber format — RS-274X, or do you prefer X2? Do you accept IPC-2581 or ODB++ instead? Separate drill files, or one with plating defined inside? Which surface finishes do you stock, and what are the lead times? What impedance tolerance do you guarantee, and will you adjust my stackup? How do you want the package delivered, and how should files be named? * For assembly: what centroid format and which rotation convention?
That last one matters more than it sounds. Rotation convention is not standardised, and a part rotated 90° the wrong way is a whole build scrapped.
A release checklist
Before sending anything:
Fabrication
- [ ] All copper layers present, count matches the stackup
- [ ] Soldermask and silkscreen for both sides, as applicable
- [ ] One closed board outline, on one layer
- [ ] Drill files present; finished vs tooling stated
- [ ] Fabrication drawing with finish, thickness, tolerances
- [ ] Impedance requirements stated if applicable
- [ ] No internal or notes layers exported by accident
Assembly
- [ ] BOM with manufacturer and MPN on every line
- [ ] DNP lines present, marked and explained
- [ ] Centroid file; DNP positions excluded
- [ ] Centroid origin matches the Gerber origin
- [ ] Rotation convention agreed with the assembler
- [ ] Assembly drawing with polarity and pin 1
Control
- [ ] Board revision stated inside the package, not only in the file name
- [ ] Release identifier and date
- [ ] Manufacturing notes included
- [ ] A manifest listing what is in the package
- [ ] Someone other than the author has reviewed it
Viewing your own output before you send it
Open the Gerbers in a viewer that is not the one that produced them. Your ECAD tool will always render its own output as intended; an independent viewer shows what the fabricator will actually see.
It takes five minutes and catches the missing layer, the open outline and the stray notes layer in one pass.
Preparing a package once is an afternoon's work. The problem arrives at the third revision, when there are three folders with similar names and the question stops being what do I send and becomes which of these was actually built.
In XKEMA the manufacturing package belongs to a PCB revision, an approved version is frozen, and two revisions of a package can be compared by their geometry.
Hardware documentation Hardware revision control PCB fabrication vs assembly: who needs which files? How to check your Gerber files