A PCB manufacturer needs enough information to build the bare board, and an assembler needs additional information to place and solder parts. These are related but different deliverables. Gerber files describe PCB layers, drill files define holes and slots, fabrication notes define process choices, and assembly files describe components and placement.
The safest approach is to build one clear fabrication ZIP for the board house and, when needed, a separate assembly package for PCBA. Before sending the fabrication ZIP, open it in the free Gerber viewer so you can confirm the actual files are present and aligned.
If you are unsure how Gerber images differ from holes, read Gerber files vs drill files before exporting. That distinction is the foundation for a complete manufacturing package.
Quick answer
For bare PCB fabrication, send Gerber layer files, Excellon drill files, a board outline, and fabrication notes. For assembly, also send a BOM, pick-and-place file, assembly drawing, polarity notes, and any stencil or process requirements.
Files for bare PCB fabrication
For a standard PCB order, the core package is the set of CAM outputs that define the physical board. The most common format is RS-274X or Gerber X2, with one image file per layer. A simple two-layer board normally includes top copper, bottom copper, top solder mask, bottom solder mask, top silkscreen, bottom silkscreen if used, and a board outline or mechanical layer. Multilayer boards also include inner copper layers in the intended stack order.
The second required piece is the Excellon drill output. Drill files list hole locations and tool diameters, including vias, through-hole pads, mounting holes, and routed slots when the CAD tool emits them that way. If your system separates plated through holes from non-plated holes, include both files and make the plating status clear.
The board outline deserves special attention. It may be a Gerber layer, a mechanical layer, or a route layer depending on your EDA tool and fab preference. It should show the finished shape, not just a drawing aid. Include internal cutouts, slots, castellations, tabs, V-score lines, or panel rails when those features are part of the order.
Fabrication notes and stackup information
Many order forms ask for material, thickness, copper weight, solder mask color, silkscreen color, and surface finish. The order form is useful, but controlled requirements should also be written in fabrication notes or a drawing when they matter. Examples include FR-4 grade, finished thickness, outer and inner copper weights, impedance requirements, controlled stackup, via tenting, solder mask expansion assumptions, gold fingers, peelable mask, carbon ink, and special tolerances.
Do not invent tolerances or capability numbers. Use the manufacturer's published capability table and quote options. Minimum trace and spacing, minimum mechanical drill, minimum laser via, copper-to-edge clearance, solder mask dam, and annular ring limits depend on process class, copper thickness, board thickness, and whether you chose a standard or advanced service.
Additional files for PCB assembly
PCBA needs the fabrication package plus component information. The BOM should list reference designators, quantities, values, footprints, manufacturer part numbers, approved alternates if allowed, do-not-populate parts, and sourcing notes. The pick-and-place file, also called centroid or XY data, should list each placed component with X/Y location, rotation, and side of board.
Assembly drawings help a human reviewer understand placement, polarity, connector orientation, pin 1 marks, and special handling. Include notes for LEDs, diodes, electrolytic capacitors, connectors, shields, thermal pads, hand-soldered parts, conformal coating, no-clean requirements, RoHS requirements, and parts that should not be washed or reflowed. Paste layer Gerbers are commonly included when a stencil is required.
Integrated manufacturing-data alternatives
Gerber plus Excellon remains the common baseline, but it is not the only option. IPC-2581 and ODB++ are modern manufacturing data packages that can bundle layer images, netlist information, drill data, stackup attributes, and component information more explicitly than a loose set of Gerber files. Many fabs accept one or both formats, especially for complex boards, but support is not universal. Confirm the accepted format before using IPC-2581 or ODB++ as your only handoff.
File list reference
| File type | Purpose | Required for fab / assembly |
|---|---|---|
| Gerber copper layers | Define conductive copper shapes on each PCB layer. | Fabrication |
| Solder mask Gerbers | Define where solder mask openings expose copper. | Fabrication |
| Silkscreen Gerbers | Define printed legend, references, polarity marks, and logos. | Fabrication when silkscreen is used |
| Board outline / mechanical | Defines finished shape, cutouts, slots, and route features. | Fabrication |
| Excellon drill | Lists hole coordinates and tool diameters. | Fabrication |
| Fabrication notes | Specify stackup, thickness, copper, finish, and special rules. | Fabrication when requirements matter |
| BOM | Lists components, quantities, references, MPNs, and sourcing. | Assembly |
| Pick-and-place | Lists component X/Y location, rotation, and board side. | Assembly |
| Assembly drawing | Shows placement intent, polarity, and special assembly notes. | Assembly |
| Paste Gerbers | Define stencil apertures for solder paste deposition. | Stencil or assembly |
Common mistakes to avoid
- Sending only Gerber layer images and omitting drill files. The fab needs both image data and hole data.
- Mixing fabrication and assembly revisions. The BOM, centroid file, and Gerbers must describe the same board revision.
- Uploading a native CAD project when manufacturing outputs were requested. Native files can be useful by agreement, but they should not replace clear CAM outputs for a normal quote.
- Leaving part polarity to assumption. Diodes, LEDs, electrolytic capacitors, connectors, and IC pin 1 orientation should be obvious in assembly drawings and silkscreen.
- Forgetting special process notes such as impedance control, gold fingers, via tenting, panelization, or no-clean assembly requirements.
Check the package before sending it
Open the fabrication ZIP in the Gerber viewer before upload. Confirm that the board outline, copper, mask, silkscreen, and drill data are all present and aligned. Then use the pre-order Gerber checklist for a final pass through naming, notes, and manufacturability checks.
FAQ
- Do I need to send native CAD project files to a PCB manufacturer?
- Usually no. For standard PCB fabrication, send manufacturing outputs such as Gerbers, Excellon drill files, and fabrication notes. Native CAD files may expose unnecessary design data and can create version ambiguity unless the manufacturer specifically requests them.
- What extra files are needed for PCB assembly?
- For assembly, add a BOM, pick-and-place or centroid file, assembly drawing, polarity notes, and any special process notes. Paste layer Gerbers are also commonly used for stencil generation.
- Can I send IPC-2581 or ODB++ instead of Gerbers?
- Many modern manufacturers accept IPC-2581 or ODB++ packages, and they can carry richer manufacturing data than separate Gerber files. Confirm support with your fab before using them as the only deliverable.
- Should the drill file be in the same ZIP as the Gerbers?
- Yes. The fab needs the drill data with the layer images, and keeping them in one clearly named ZIP reduces the chance that holes, slots, or NPTH data are missed.