Releasing Gerber Files and Fabrication Data to a PCB Manufacturer
Releasing a board for manufacture means handing a fabricator a set of files that describe the copper, the solder mask, the legend and the holes without ambiguity. Almost every format in that set is a convention rather than a standard drawing, which is why the same design can produce a clean build from one release and a scrap lot from another. The differences are usually settings rather than geometry, and they are all decided in the last hour of the project.
What the Release Contains
A complete package has four parts, and each one goes to a different place in the factory.
The layer images define the copper, the mask and the silkscreen. They are called Gerber files in common usage, and the whole electronics assembly industry reads them, so a fabricator can accept them from any design tool without a native file.
The hole data defines every drilled feature with its size and position. The NC drill file is what the drilling programme is built from, and a plated hole and a non-plated hole have to be distinguished in it, because they are drilled on different schedules and finished differently.
The IPC netlist is a text description of what should connect to what. It is not needed to build the board, but it is the cheapest way for the fabricator to check the artwork against the design intent, because a netlist comparison finds opens and shorts before the board is etched.
The pick and place file is the assembly data: reference designator, position and rotation for every part. It carries no board geometry, so it is easy to generate and easy to generate wrongly.
Settings That Decide Whether the Data Is Usable
Units and format come first. Imperial units with a two by four format, meaning two digits before the decimal point and four after, are still the safest choice for a fabricator, because that is what most drilling and imaging equipment expects. A file released in metric with an unusual precision may be readable, but every conversion is a chance for a mistake.
The layer selection is the next trap. Generating only the layers that are used avoids publishing empty layers, but the selection has to be reviewed, because a design that keeps a mechanical outline layer unplotted loses the board contour, and a negative plane layer that is left out produces a board with no power plane. The list is worth reading once against the stack-up rather than being accepted as generated.
Mirroring must be off for every layer. A mirrored silkscreen or copper layer is a plausible-looking file that produces a board that cannot be assembled, and the error is invisible in a viewer that flips the view.
The aperture format matters for the same reason. The modern approach embeds the aperture definitions in each file, so the file is self-describing and the fabricator does not need a separate aperture list that can be mismatched with the data. A design released in the older format with a separate aperture file is one transaction error away from a wrong build.
Film size is the setting that most often causes a silent defect. If the calculated plotting area is too small, the tool clips features at the edge of the panel or refuses to plot them, and what arrives at the fabricator is a board with missing copper near the border. Enlarging the film size beyond the board outline removes the risk, and it costs nothing.
Drill Data and the Legend
The drill drawing is generated with all used drill pairs, so every via and hole type appears. The useful convention here is a drill legend printed on a documentation layer, which lists each hole size with its count and its symbol. Placing it on the drawing layer rather than on the production layers keeps it out of the artwork, and the legend text has to be small enough that the legend does not overlap the board outline. A legend around 30 mil high with a 5 mil stroke reads clearly at the scale a fabricator prints.
The legend also gives the fabricator a quick check. If the legend says there are four sizes and the drill file contains two, something in the release is wrong, and it is found before the drill is programmed rather than after.
The Assembly Data
The pick and place output is generated from the same database, but its settings are independent. The unit should be millimetres for assembly, because placement programmes are metric and a file in inches adds a conversion step. The coordinate origin should be the same origin the design uses for its own documentation, and it should be stated in the file header, because a placement programme that assumes a different origin will place every part offset by a fixed distance.
The rotation convention is the part that most often goes wrong. Different tools express a rotation relative to a different reference, and a part rotated by ninety degrees in the wrong convention presents as a systematic orientation error on one package type. The fix is a sample placement check on the first board, and the review of the data package before release is what makes that check short. Our PCB manufacturing review includes a comparison between the placement file and the assembly drawing for exactly this reason.
Packaging and Revision Control
What is sent is a folder, and the folder should be organised so that a fabricator can see the revision at a glance. A named project folder containing the layer images, the drill files, the netlist, the placement file and a readme with the stack-up, the surface finish, the board thickness and the impedance requirements is enough for most builds.
The revision number has to be inside the data as well as in the folder name. A silkscreen that carries the board revision is a small change that prevents the most expensive failure in this area, which is a fabricator building an older revision because the folder was reused. Our order process checks the data package against the purchase order before any tooling is made, precisely because this error is common.
Where the design is still moving, the release should be planned rather than improvised. A prototype where the layout changes weekly needs a data package convention that is quick to produce and unambiguous to read, and our rapid PCBA prototyping service is set up around short, repeatable releases rather than one-off transfers.
Checking the Package Before It Leaves
The last step is a read-through of the fabrication data as a fabricator would read it, without the design open beside it. A viewer that shows each layer on its own confirms that the copper, the mask and the legend are each complete; a drill chart confirms that every hole size listed is one the shop can produce; a stack-up sheet confirms that the layer count in the drawing matches the layer count in the files. This is the point where a mismatch between the design and the shop capability is still a phone call, and where a missing layer is still a regeneration rather than a scrapped lot. Our capability review is written to be read at that moment.
FAQ
Do I need to send the design source files? No. A complete Gerber and drill package is sufficient for fabrication, and the placement file covers assembly.
What does the IPC netlist add? It lets the fabricator compare the artwork against the intended connectivity and detect opens and shorts before manufacturing, which is cheaper than finding them on the finished board.
Which settings cause missing features near the board edge? A film size that is too small for the board, which clips the plotted area. Enlarging the film size removes the risk.
