Gerber Files for PCB Manufacturing: Reference Guide
Complete reference for PCB fabrication data packages — RS-274X Gerber format, Excellon drill files, ODB++, IPC-2581, fabrication notes, and how to specify board parameters correctly when ordering from a Chinese PCB factory.
The Gerber package is the set of files you send a PCB assembly factory to manufacture your board. An incomplete or ambiguous Gerber package results in the factory making assumptions — and factory assumptions often produce boards that are technically “as drawn” but functionally wrong. Knowing exactly what to include and how to specify it eliminates the most common PCB fabrication errors. Getting this right before sourcing a manufacturer saves costly revision cycles later.
Overview
PCB fabrication data has evolved through three main formats: legacy Gerber (RS-274D, obsolete), extended Gerber (RS-274X, universal), and newer formats like ODB++ and IPC-2581 that include netlist and assembly data in a single file. Most Chinese factories accept RS-274X as their primary input; a growing number prefer ODB++ for complex boards. IPC-2581 adoption is increasing in automotive and aerospace but remains uncommon in contract manufacturing.
The Gerber package describes geometry only — what copper is where, where solder mask openings are, where silkscreen markings go. It does not inherently describe what materials to use, what finish to apply, or what quality standards to meet. That information goes in fabrication notes, stackup drawings, and your purchase order. The factory’s job is to manufacture what the Gerber says; your job is to make sure the Gerber plus notes says what you actually want.
What to Include in the Fabrication Package
Mandatory files:
| File | Description | KiCad Export | Altium Export |
|---|---|---|---|
| Copper layers | Top, bottom, inner layers | Cu_F, Cu_B, In1.Cu, etc. | GTL, GBL, G1, G2, etc. |
| Solder mask layers | Top and bottom (inverted from pads) | Mask_F, Mask_B | GTS, GBS |
| Silkscreen layers | Top (bottom optional) | SilkS_F | GTO |
| Board outline | Mechanical boundary | Edge.Cuts | GM1 or GKO |
| Drill file | Through-hole and via drill positions | .drl (Excellon) | .drl (Excellon) |
| Drill map | Visual reference for drill sizes | .gbr drill map | DRL |
| Fabrication notes | Text document with all specs | Manual | Manual |
Recommended additions:
- Assembly drawing (reference designators, component outlines)
- Impedance stackup drawing (for controlled-impedance boards)
- IPC-4761 specification for via fill type (if applicable)
- 3D model (STEP file) for mechanical check
Gerber Format: RS-274X
Always export RS-274X (extended), never RS-274D (obsolete). The difference: RS-274X includes embedded aperture definitions in the file header, so the factory’s CAM software can parse the file without a separate aperture list. RS-274D requires a separate D-code file that almost no modern CAM system reads correctly.
In RS-274X, verify:
- Units: millimeters (recommended) or inches — state explicitly in fabrication notes, do not rely on file header alone
- Coordinate resolution: use at least 4.6 decimal format (4 digits before decimal, 6 after) for millimeter files to avoid rounding errors on fine-pitch pads
- Gerber polarity: dark = copper (standard), light = mask opening — confirm with factory if non-standard
Excellon Drill File
Drill position files use Excellon format. Common issues:
- Units: Excellon files can be metric or imperial, and the header declaration is sometimes missing or ignored. Always state drill units in your fabrication notes and verify the factory acknowledges them.
- Drill table: include a drill table as a Gerber overlay or PDF showing each drill symbol, finished hole size, drill count, and plating status (PTH vs NPTH)
- Minimum hole size: confirm with factory — standard capability is 0.30 mm finished, some factories do 0.20 mm but at premium cost
- Slot routing: Gerber outline file or separate rout file for slots; Excellon format for slots is less standardized — verify factory’s preferred format
ODB++ Format
ODB++ (Open Database++) is a directory structure containing all board data in a single compressed archive. Advantages over Gerber: layer registration is exact (no separate outline file needed), drill and copper data are in one consistent coordinate system, netlist is included (enables electrical DRC at the factory), component library data is embedded. If your factory’s CAM system supports ODB++ (most modern Valor/Genesis systems do), prefer it for complex multi-layer boards. Export from Altium natively; KiCad requires a plugin.
IPC-2581
XML-based format combining all board data plus full netlist. Best for boards requiring strict traceability and where the factory will run DFM/DFA analysis in their CAM system. Increasingly required by automotive Tier 1 suppliers and aerospace. For most commercial electronics, RS-274X or ODB++ is sufficient.
Fabrication Notes — What to Specify
This is the most important document in the package. Every parameter not in the Gerber geometry must be written here.
Required parameters:
Layer count: 4
Board thickness: 1.60 mm ± 0.15 mm
Board dimensions: 85.0 × 60.0 mm
Copper weight: Outer layers 1 oz (35 µm), Inner layers 0.5 oz (17.5 µm)
Minimum trace/space: 0.10/0.10 mm
Minimum drill (finished hole): 0.30 mm
Via fill: None (open via, tented with mask)
Surface finish: ENIG — Nickel 3–6 µm, Gold 0.05–0.10 µm per IPC-4552A
Solder mask: Green, LPI, both sides
Silkscreen: White, top side only
Board material: Shengyi S1141 high-Tg FR4, Tg ≥ 170°C, Td ≥ 310°C
UL marking required: Yes (UL file number on board)
Impedance control: Yes — see stackup drawing
Layer 1: 50 Ω single-ended, 100 Ω differential (referenced to Layer 2)
Quantity: 500 panels (2 boards per panel, V-score)
IPC Class: Class 2 per IPC-6012
Test method: E-test (100% continuity and isolation)Solder mask expansion: default factory expansion (typically 75–100 µm per side from copper pad edge) may be too large for 0.4 mm pitch QFP footprints. Specify “solder mask expansion 50 µm from pad edge” if you have fine-pitch components.
Surface finish thickness: ENIG thickness varies significantly between factories. Specify per IPC-4552A: Ni 3–6 µm, Au 0.05–0.10 µm. Thinner Au (<0.05 µm) causes solderability issues; thicker Ni (>6 µm) affects drill registration on fine vias.
Naming Conventions
Use descriptive, version-controlled filenames. Bad: copper_top.gbr. Good: PCB_SmartSensor_v1.2_2026-05-08_Cu_F.gbr. The full package should be: PCB_ProjectName_vX.Y_YYYY-MM-DD.zip containing all files in a flat directory structure (some factories cannot handle nested subdirectories in zip archives).
Design Rule Check Before Sending
Run a DRC in your CAD tool before exporting. Common DRC-clean but fabrication-problematic issues:
- Copper features outside board outline (some tools don’t catch this)
- Board outline not a closed loop (factory’s CAM system may fail to parse it)
- Drill hits without annular ring on inner layers
- Silkscreen text under components (invisible after assembly, wastes silkscreen pass)
- Missing or asymmetrically placed fiducial markers
Also run a visual Gerber check in a standalone Gerber viewer (Gerbv, FAB3000, or your CAM tool’s viewer) before sending. The visual check catches layer polarity errors (mask inverted, copper missing) and coordinate unit errors that DRC misses.
What to Specify When Ordering from China
- Request DFM report before production start: most factories provide a free DFM check within 24–48 hours — review it and respond in writing before approving production start
- Confirm Gerber units: state units explicitly in fabrication notes AND verify factory confirms them in their DFM feedback
- Impedance coupon requirement: for controlled-impedance boards, require an impedance coupon on each panel (or every N-th panel) and specify that production panels must measure within ±10% of target before proceeding
- E-test (electrical test): for any volume over 50 boards, specify 100% electrical continuity and isolation test — adds $0.05–0.20/board but catches opens and shorts from fabrication before assembly
- First article approval: require factory to submit first-off-tool board for your approval (or your inspector’s approval) before proceeding to full production
Common Issues
Drill file unit mismatch: Factory interprets inches as millimeters. All drill hits are off by 25.4×. Every hole is in the wrong position. The board is scrap. This happens more often than it should. Prevention: include a drill table PDF with finished hole sizes in both mm and inches, and verify the drill positions match your copper pads in the DFM feedback.
Missing board outline: Factory extrapolates board edge from copper keepout zones or the bounding box of all Gerbers. Result is often a board 0.5–1.0 mm oversized, which may not fit the enclosure. Always include a dedicated Edge.Cuts or mechanical layer with a clean closed outline.
Silkscreen encroaching on pads: Factory removes silkscreen from pad areas per IPC-7527 (silkscreen must not cover solderable surfaces), but the clipping changes silkscreen readability — reference designators get partially clipped. Run silkscreen DRC to push text off pads before export.
Related Resources
- PCB Substrate Materials — material parameters that go in fabrication notes
- DFM Guidelines — design rules to verify before Gerber export
- SMT Assembly Process — what happens to the board after fabrication
- Factory Audit Checklist
- Supplier Sourcing & Matching
- PCB Manufacturing & SMT Sourcing
- PCB Assembly China Buyer’s Guide