A factory builds from files, not from your design project. What you export is what you get, so the export is a step of the design, not an afterthought. This article lists what each file must contain, how to export it from the common tools, and what goes wrong most often.
The files, one by one
Gerber files (the copper, mask and legend images)
A Gerber file is a 2D image of one layer. You send one file per layer:
- each copper layer (top, bottom, and every inner layer),
- solder mask top and bottom (the openings where copper is left uncovered),
- legend or silkscreen top and bottom (the printed text and outlines),
- solder paste top and bottom, if the stencil is made from your files,
- the board outline.
Use the current format, RS-274X (extended Gerber), or its newer variant Gerber X2, which can carry layer function in the file. The old format without embedded apertures (RS-274D) is not acceptable. Check that the file units and the number of decimals are set in the file; a file that is read in the wrong unit appears ten or twenty-five times too large or too small.
The drawing pulls a board apart into the layers that become files. Each file is an image of one layer alone.
- Legend (silkscreen): the printed outlines and marks, kept off the pads.
- Solder paste: where the stencil lets paste through. Its openings are on pads only.
- Solder mask: the coating. The file shows where it is open, not where it is, so the openings are at the pads.
- Copper: pads, tracks and the ring round a via. There is one file for each copper layer; one is drawn here.
- Drill: the position and size of every hole. It is a list of holes, not an image.
- Outline: one closed shape for the board edge, with cut-outs and slots as shapes of their own.
On one pad these files meet. This cross-section shows a pair of pads and the three layers that touch them, which is why they are separate files.
- The pad is copper, from the copper file.
- The mask opening is larger than the pad, so a ring of bare board shows round the copper.
- The mask between two pads is a narrow web. If it is too thin to hold, it is lost and solder can join the pads.
- The stencil opening, from the paste file, is a little smaller than the pad, so the paste lands inside it.
- The legend sits on the mask, away from the pads. Ink on a pad stops solder.
Drill files
Drill data lists the position and diameter of every hole, usually in Excellon format. Send plated holes (vias, component holes) and non-plated holes (mounting holes) separately, or make sure the file says which is which. Slots must be in the drill or the outline file in a form the factory can read; say in a note if you are unsure.
The board outline
The outline is one closed path that describes the board edge. Internal cut-outs are separate closed paths. An outline that is not closed, or that is drawn on several layers, is a frequent cause of questions. Draw it on its own layer, with a single line width.
The BOM
A table of the parts: reference designators (R1, C4, U2), quantity, value, footprint, and the manufacturer and manufacturer part number. Writing a BOM a factory can buy covers this in detail.
The placement file
Also called pick-and-place or centroid file. For each reference designator: X and Y position, rotation, and which side the part is on. Two traps are common. The origin may differ from the Gerber origin, and the rotation of a footprint may follow a different convention from the one the machine library uses. A good BOM and a bad placement file still gives wrong boards, and the factory cannot tell without a picture, so send an assembly drawing or a PDF of each side as well.
Exporting from common tools
The menu names change between versions, so treat this as a map, not a manual.
| Tool | Gerber and drill | Placement file | BOM |
|---|---|---|---|
| KiCad | Plot dialog in the PCB editor (File, Fabrication Outputs, Gerbers), then Generate Drill Files | File, Fabrication Outputs, Component Placement | Export from the schematic editor; add manufacturer and part-number fields to the symbols first |
| Altium Designer | File, Fabrication Outputs: Gerber Files and NC Drill Files | File, Assembly Outputs: Generate pick and place files | Reports, Bill of Materials |
| Eagle (and the Fusion electronics editor) | CAM Processor with a Gerber and an Excellon job | ULP or script that writes a placement list | ULP or the BOM export |
| EasyEDA | Export, PCB Fabrication File (Gerber) | Export, Pick and Place File | Export, BOM |
After exporting, open the files in a Gerber viewer that is not part of your design tool, and compare what you see with the design. A free viewer is enough. This single step catches most of the mistakes below.
The ten most common file mistakes
- A layer is missing. For example the bottom mask, or the drill file, or one inner layer.
- The outline is open or in the wrong place. The factory has to guess the board edge.
- Wrong units or scale. The board shows up at the wrong size.
- The bottom side is mirrored. Some export settings mirror the bottom layers, and a mix of mirrored and unmirrored layers in one set gives a board whose bottom copper does not match its bottom mask or its drill holes. Export all layers with the same settings and look at the result in a viewer.
- Holes do not land on their pads. The drill file uses a different origin or a different format from the Gerbers.
- Tracks or gaps thinner than the process makes. Every manufacturer has a minimum for track width, spacing, hole size and annular ring (the copper ring around a hole).
- Copper too close to the board edge. Routing the board edge cuts into copper that is too near.
- Legend on pads. Text over a pad is removed, or ink on a pad stops solder from wetting.
- No solder mask between fine-pitch pads. The mask web between pads can be too thin to hold and is left out, which invites solder bridges.
- BOM and placement file disagree. A reference designator is in one and not in the other, or the footprint in the BOM is not the footprint on the board.
Name things so that no one has to guess
Use clear file names or a single archive in which every file has the layer in its name or its extension. Include a short readme with the board thickness, the number of layers and the finish you want, and what you want for anything unusual: gold fingers, blind vias, controlled impedance.
What a file check can and cannot tell you
An automated check can read the files and find what is missing, inconsistent or outside the process: an open outline, a mirrored layer, a hole missing its pad. It cannot tell whether the circuit works, whether the part you chose is right, or whether the schematic matches the board. That stays your job and your design review's.
How this shows up when you order here
Upload a single archive at the upload page; what the check covers is on the file check page. The 25 checks are named in plain language in the result, with how many places each problem occurs and the limit it was measured against. The limits in force are on the capabilities page. If a check could not run, for instance because assembly files are not uploaded yet, the result says so instead of showing a green mark. An engineer confirms every order before production.
For the list of design mistakes organised by check, read Design for manufacture: the mistakes we see.