Every PCB order starts with a set of files that most designers never open again after clicking export. The Gerber package is what the fabricator reads. It decides where copper sits, where the solder mask opens, where every hole lands, and where the board ends. If something in that set is wrong, no amount of process control further down the line can fix it.
This guide covers what goes into a Gerber package, which layers cannot be left out, the mistakes that cause the most rework, and how to export a clean set from KiCad, Altium, and EasyEDA. The review that happens after the files reach the factory is a separate step, covered in our walkthrough of the PCB DFM review process.
What a Gerber File Contains
Gerber started in the 1960s as the control language for photoplotters, machines that exposed PCB artwork onto photographic film. The machines are gone and the format is not. What you export today is Extended Gerber, usually called RS-274X, and it differs from the original in one way that matters: the aperture definitions travel inside the file. Older RS-274D output needed a separate aperture list, so a missing list left the fabricator guessing at pad sizes and trace widths.
A single Gerber file describes a single layer. Inside it you find coordinate moves, draw and flash commands, aperture definitions, and a unit declaration. That unit declaration matters more than it looks. A file plotted in inches but opened as millimetres comes out 25.4 times too large, and the receiving engineer has no way to know whether the design was meant to be that size or the unit was simply mislabelled. The specification is maintained today by Ucamco, and the X2 revision added attributes that label each file with its layer function, which removes most of the guesswork at the factory end.
The Layers a Fabricator Needs
Picture the package as a stack of transparencies, one for each physical layer of the board. A two-layer job needs fewer files than a six-layer one, but the categories stay the same:
- Copper layers: top, bottom, and every inner layer. Inner plane layers included, even when they are almost entirely one pour.
- Solder mask: top and bottom. These files describe the openings, not the coating itself.
- Silkscreen: top and bottom wherever it is used. Reference designators, polarity marks, pin 1 indicators.
- Paste mask: top and bottom. Only needed if the board will be assembled, since this layer drives the stencil.
- Board outline: one closed profile. This is the file that tells the fabricator where to route.
- Drill data: normally a single Excellon file. Strictly speaking the drill file is Excellon rather than Gerber, though it belongs in the same package and almost always ships with it.
If you have not settled how many copper layers the design needs, our guide to PCB layer types and their functions covers what each one does before the export stage.
The Mistakes That Stop a Job
Most rejected file sets fail for the same handful of reasons, and they are packaging errors rather than design flaws. Each one costs a day or more while the job sits in a queue waiting for an answer.
Units and Coordinate Format
A board plotted in inches and opened as metric will not fit any panel. The coordinate format can do similar damage with no unit error at all. Gerber writes positions with a fixed number of integer and decimal digits, and the leading or trailing zero suppression has to match what the reader expects. Get that pair wrong and every feature shifts by a factor of ten, which usually looks like a board with pads scattered across the panel rather than a clean fail.
An Outline That Does Not Close
The profile has to be one closed contour on one layer. Two arcs that almost meet will not route, and neither will a leftover segment parked on a mechanical layer or a corner drawn as a separate polyline. Some fabricators will email and ask. Others will panelise to the bounding box and ship you a board with square corners where you designed a radius.
Drill Data Out of Alignment With the Copper
Drill files are generated in a separate step from copper, and that step has its own origin setting. Plot the copper from an auxiliary origin and the drill from an absolute origin, and every hole lands off centre. The board passes electrical test and still fails mechanically, because the annular ring on one side is now a sliver.
Slots Recorded as Round Holes
Oval slots, plated cutouts, and castellated edges fail the same way. If a slot exports as a drill hit at one end, the fabricator drills a round hole and your connector no longer seats. Slots need a routed representation, either a G85 command in the drill file or a contour on a mechanical layer with a note attached.
Silkscreen Printed Over Exposed Copper
Ink printed across a pad gets clipped by the mask opening, so the legend vanishes exactly where the assembler needs to read it. Reference designators are the usual casualty, and rework starts with someone hunting for a part they cannot identify.
Mirrored Bottom Layers
Bottom copper viewed from above instead of from below produces a plausible-looking file in which everything is reversed. Pad 1 of a connector ends up on the wrong side, and the error survives until the assembly house tries to place the part.
Exporting Gerber Files from KiCad
- Open the board file, then go to File > Fabrication Outputs > Gerbers (.gbr).
- In the plot dialog, select the layers you need: F.Cu, B.Cu, any inner copper, F.Mask, B.Mask, F.Silkscreen, B.Silkscreen, F.Paste, B.Paste, and Edge.Cuts.
- Pick an output folder, set the format to Gerber, set units to millimetres, and enable the Protel-style extensions. That produces .GTL, .GBL, .GTS, .GBS, .GTO, .GBO, and .GM1, so the fabricator can identify each file without opening it.
- Click Plot. The files appear in the folder you chose.
- Run Generate Drill Files from the same menu, choose Excellon and millimetres, and decide whether plated and non-plated holes go into one file or two. Keeping them separate makes the check easier.
KiCad takes the outline from Edge.Cuts, so confirm the profile lives on that layer and closes before you plot. If you only need to get Gerber files out of KiCad for a quick quote, steps 1 through 4 give you the artwork and step 5 gives you the drill data. A package without the drill file cannot be built, so run all five.
Exporting from Altium and EasyEDA
In Altium, use File > Fabrication Outputs > Gerber Files. On the Layers tab, take the used layers or tick them by hand, and enable the option that includes unconnected mid-layer pads if the design has any. On the Output tab, choose RS-274X with 2:4 or 2:5 format. Then run NC Drill Files as a second operation. The default film in a new project often carries mechanical layers you did not intend to publish, so look at the layer list before plotting rather than after.
In EasyEDA, the standard edition exports under Fabrication > Gerber, while the pro edition puts it under Manufacture > Export Gerber. Both produce a zip that should contain the copper, mask, silk, and outline files. Open the zip and count them. A common slip is exporting Gerbers from one menu and drill data from another, then sending only half the package.
Check the Files Before You Send Them
GerbView ships with KiCad and reads the whole set at once. Any Gerber viewer will do the same job, and what matters is loading every file, then hiding them one by one. You are looking for four things: an outline that closes, drill hits sitting centred on their pads, mask openings slightly larger than the copper they expose, and silkscreen clear of every opening.
Compare the hole sizes against your own drill table as well. Our reference on PCB drilling dimensions covers hole diameter and the pad size that has to surround it. The aspect ratio is the other half of that decision: a 0.2 mm hole through a 1.6 mm board reaches 8:1, which is roughly where standard capability ends.
Another check catches what the others miss: count the drill hits in the file and compare that number with the design. A board with twelve vias should report twelve hits. If the count is off, a tool did not export rather than the design being wrong.
What to Send Alongside the Gerbers
For bare fabrication, the Gerber set plus the drill file is enough. For assembly, the package needs more:
- A BOM with manufacturer part numbers and reference designators, so sourcing can proceed without a second email.
- A pick-and-place file with the rotation convention stated, since 0 degrees means different things in different tools.
- A stack-up and material callout when impedance control applies, instead of letting the fabricator infer it from the copper.
- Any special process notes: controlled-depth drilling, press-fit holes, edge plating, or a required surface finish.
If the stack-up is still open, our guide to PCB stack-up structure and design rules covers how layer order and dielectric thickness affect both signal behaviour and price. For boards that go straight to assembly, the inputs we need for PCBA assembly and testing are the same list with the centroid file added.
From Gerber to PCB: The Manufacturing Route
Once the file set is clean, the rest of the route is manufacturing rather than data. The artwork goes to a photoplotter or a direct imaging system, the drill program runs on its own machine, and the two have to agree before the first panel is worth building. Errors at this stage are cheap to fix in software and expensive to fix in copper.
If you want to see how the fabrication steps follow on from the file set, our overview of printed circuit board manufacturing walks through the sequence from inner layer imaging to final test. And if this is a first build rather than a production run, the notes on PCB prototype process and pitfalls cover what tends to go wrong when quantities are small.
Send us the Gerber package and we will check it against our process capability before quoting. The reply usually comes back with a question about one layer, and it is better to answer that question now than after the panel is etched.
