How Gerber Files Work When Manufacturing PCBs in China

Gerber files are the manufacturing data a Chinese PCB fab builds your board from: a flat image of one board layer per file — copper, solder mask, silkscreen, drill holes — in the plain-text RS-274X format, usually extended as Gerber X2. Everything geometric lives in the Gerbers; board thickness, material, copper weight, and surface finish come from the order form.

That split is why Gerber exports stall so many orders: when the files are ambiguous — a missing outline, two competing outlines, a drill file in the wrong units — the fab cannot guess, so it stops and asks. These engineering questions, or EQs, cost days across time zones.

The fix sits almost entirely in the export step, before you upload anything. Buyers who order through a sourcing agent usually hand this step over: CN Ally's product sourcing team checks the file set and answers EQs with the fab directly.

What does a Gerber file actually contain?

A single layer's artwork, nothing more: a list of vector drawing commands in 7-bit ASCII text. Select an aperture (a shape — round, square, rectangular, or custom), move to a coordinate, then flash the shape or drag it to draw a line. Stack every layer's file in register and you get the complete picture of the board.

What is not in the files matters just as much: shapes and nothing else. No board thickness, no material, no copper weight, no surface finish, no net names (in X1), no part numbers. Two boards from identical Gerbers can be 0.8 mm or 2.0 mm thick, two-layer or four-layer, HASL or ENIG — all decided by the order form, not the data.

The format is maintained by Ucamco. The modern extension, Gerber X2, adds attribute commands that let a file declare metadata — "I am the top copper layer," "this pad is an SMD pad" — while staying fully backward compatible: an older X1 reader renders the same image and ignores the attributes. KiCad exports X2 by default, which is why modern fabs can auto-identify layers instead of demanding exact filenames.

RS-274X vs Gerber X2: which format should you send to China?

Either one — every Chinese fab accepts RS-274X, and Gerber X2 is its backward-compatible upgrade. If your EDA tool offers X2 output, use it; plain RS-274X works fine too.

Feature · RS-274D · RS-274X · Gerber X2

• Aperture definitions: Separate external file · Embedded in each file · Embedded in each file
• Metadata / attributes: None · None · File function, pad type, net names (TF, TA, TO, TD)
• Status: Revoked by Ucamco in 2014 · Active, universally supported · Active, recommended
• EDA tool support: Rarely offered · Universal · Growing

RS-274D, the original "standard Gerber," kept aperture definitions in a separate file; if the two files disagreed, the fab built the wrong shapes. Ucamco revoked the standard in 2014, and reports that fewer than 2% of jobs still arrive in the old format.

The practical difference between RS-274X and X2 shows up at the fab's CAM station. With plain X1, the engineer assigns each file to a layer manually, usually by filename; with X2 attributes, the file declares its own function, so the import assigns layers automatically and flags conflicts. Either way, the image the fab builds is identical.

Which files does a Chinese PCB fab actually need?

For a standard two-layer board: top and bottom copper, top and bottom solder mask, top and bottom silkscreen, exactly one board outline, and the drill file. Each inner copper layer on a multilayer board adds one more file.

Extension · Layer · What it defines

• .GTL: Top copper · Traces, pads, pours on the top side
• .GBL: Bottom copper · Traces, pads, pours on the bottom side
• .G2L, .G3L…: Inner copper · One file per inner layer on multilayer boards
• .GTS: Top solder mask · Openings where the top stays free of mask
• .GBS: Bottom solder mask · Openings where the bottom stays free of mask
• .GTO: Top silkscreen · White printed legend on the top side
• .GBO: Bottom silkscreen · White printed legend on the bottom side
• .GTP / .GBP: Solder paste · Stencil apertures — only needed with assembly
• .GKO: Board outline · The routed shape of the board (Edge.Cuts)
• .drl / .txt / .xln: Drill data · Excellon NC drill: hole positions and sizes

First, the solder mask files define openings, not the mask itself: anything you draw on the mask layer is an area the fab leaves uncovered. Drawing the full board shape on the mask layer would strip the mask off the entire board. Second, the outline layer must be one single closed contour — open polylines are the most common reason a fab reports that it cannot determine the board dimensions. Third, drill data is technically a separate Excellon file, not a Gerber, and many fabs want plated and non-plated holes in separate files.

Filenames follow a Protel-era convention (.GTL, .GBL, and so on); KiCad's "Use Protel filename extensions" option makes its exports match. With X2 attributes the exact names matter less, but consistent naming still speeds up review. Zip the whole set — one archive per board revision — and keep non-manufacturing layers (fabrication notes, courtyard, drawings) out. Extra layers do not get ignored quietly; they generate questions.

How do you export Gerbers from KiCad, Altium, and Eagle?

Every EDA tool has a fabrication-output dialog that plots the same layer list — copper, solder mask, silkscreen, board outline — then drill files as a separate step. The menu paths differ; the layer list does not. Run a design rule check first, and export from the exact revision you intend to order.

KiCad

In the PCB editor, go to File → Fabrication Outputs → Gerbers, select the copper layers, both mask layers, both silkscreen layers, and Edge.Cuts, tick "Use Protel filename extensions," and click Plot. Then go to File → Fabrication Outputs → Drill Files and generate the Excellon drill file in millimeters into the same folder. KiCad exports X2 with attributes, so layer identification is usually automatic.

Altium Designer

Go to File → Fabrication Outputs → Gerber Files, confirm the layers, and generate; drill data comes from File → Fabrication Outputs → NC Drill Files. Altium supports RS-274X with X2 attributes, so the export needs no post-processing — but verify the plotted output in a viewer rather than trusting the dialog.

Eagle / Fusion

Open the CAM Processor, load a Gerber 274X job file (gerb274x.cam), and click Process Job. The processor writes each layer — copper, silkscreen, solder mask, outline — plus the drill file into the project folder. Check that the job includes the outline layer; a CAM job inherited from an old project sometimes omits it.

Whichever tool you use, the last step is the same: load every file into a free Gerber viewer and look at it. Confirm the outline is correct, the layers line up, drill holes sit on their pads, and no silkscreen overlaps a pad. Five minutes in a viewer catches most of the mistakes in the next section.

What are the most common Gerber export mistakes?

A missing board outline, by a wide margin — then duplicate outline layers, a missing or mismatched drill file, silkscreen over pads, and specs that contradict the order form.

1. No board outline. Without it the fab cannot determine the board's dimensions and the order stops immediately — a missing outline sits at the top of fabrication-hold checklists, including EDN's rundown of why assembly jobs go on hold.
2. Two outlines, or non-manufacturing layers in the zip. Sending a keep-out layer or a second outline forces the fab to ask which one is real — there are forum threads of orders suspended over exactly this. The fix is one outline only.
3. Drill file missing or in mismatched units. Holes are drilled from the Excellon file alone; if it is absent or its units disagree with the Gerbers, the fab cannot verify hole sizes or plating.
4. Silkscreen overlapping pads. Anything drawn over a copper pad gets clipped by the fab. Keep silkscreen clear of all pads.
5. Solder mask polarity confusion. Because mask files define openings, an inverted mask layer leaves pads covered and everything else exposed. If your pads come back masked, this is the first file to check.
6. Stale files. Gerbers exported from an older revision than the current design are a quiet source of wrong boards — re-export after every layout change and name the zip for the revision.
7. Conflicting fabrication specs. Thickness, copper weight, or surface finish stated differently in the notes and the order form means the fab has to ask which is correct. Make the documents agree before you upload.

How does a Chinese fab review your files?

After upload, the fab's CAM engineers check your files against its process capabilities. If anything is ambiguous, the order goes on hold and the fab sends engineering questions — EQs — which you must answer before production starts.

The review has two stages. An automated pre-check parses the archive, identifies layers, and renders a preview — this catches missing files and unreadable data. Then an engineer reviews the design itself: outline integrity, trace and space widths against the fab's capabilities, annular rings, drill sizes, impedance requirements, and whether the panelization instructions make sense. Typical EQs ask you to confirm the outline, clarify hole plating, approve silkscreen clipping, or choose a stackup for impedance-controlled layers.

Replies go through the order system or email, and each round trips across time zones. Two habits keep this fast: answer precisely, naming the file and layer, and when a file needs fixing, re-export and resend the complete zip rather than a single replacement file. Multiple versions of the same file in circulation is itself a documented cause of confusion.

This is also where fab quality varies most. A thorough review that asks sharp questions is a good sign; a fab that silently "fixes" your data to fit its process is not. Vetting the fab's engineering discipline before a production run is cheaper than discovering its habits afterward.

Panelization basics: V-score, tabs, and mouse bites

Panelization groups multiple boards onto one manufacturing panel for efficient processing and assembly. Simple rectangular boards get V-shaped score grooves along their edges; irregular shapes get routed tabs weakened by perforations called mouse bites.

Method · How it works · Best for · Watch out for

• V-score: V-shaped grooves scored into the panel along board edges · Rectangular boards, high volume · Straight edges only; can weaken very thin boards
• Tab routing + mouse bites: Boards joined by small tabs with rows of tiny drilled holes · Irregular shapes, connectors near the edge · Needs a ~2.0 mm routing channel; leaves small burrs
• Laser cutting: Precision cutting with minimal stress · Dense or high-value boards · Expensive and uncommon at prototype fabs

Mouse-bite dimensions follow rough industry conventions — holes around 0.5–0.6 mm in diameter, spaced 0.7–0.8 mm center to center, five to eight per tab, at least 0.30–0.50 mm from copper and 1.5 mm from the nearest component — documented in JLCPCB's mouse-bite guide for its own process. Keep copper at least 0.2 mm back from any routed edge so the router bit does not expose it.

You do not have to panelize the board yourself: most Chinese prototype fabs panelize single-board orders automatically, adding their own tooling rails and fiducials. Do it yourself when the shape is unusual, when the panel must fit your assembler's line, or when fragile sections need specific depaneling treatment. Mixing several designs on one panel usually costs extra for the added CAM work — for volume, one design per panel is safer.

What happens when the files are wrong?

The normal outcome is an EQ hold: the order pauses, you clarify or re-export, production starts. It costs days, not boards. The dangerous outcome is a fab that modifies your Gerbers to meet its own clearances without telling you — engineers have reported receiving unusable boards after exactly that. Never authorize a fab to "just fix" your files without seeing the modified data back: ask for the adjusted files, review them in your viewer, and approve the change explicitly.

If wrong boards do arrive, your exported file set is the evidence of what was sent versus what was built. That is the moment incoming quality control earns its keep — measuring boards against the Gerber data before they ship, rather than discovering the problem on your assembly line.

Frequently asked questions

Can I send my native CAD file (.kicad_pcb, .brd, .PcbDoc) instead of Gerbers?

Some prototype fabs accept native files and generate the Gerbers themselves, but Gerbers remain the universal handoff: any fab can build from them, the export is deterministic, and you keep control of what gets manufactured. For volume orders, a Gerber package is expected.

Do I need paste layers for a bare-board order?

No. Paste layers define the stencil apertures used during assembly; on a bare-board order they serve no purpose and can prompt an unnecessary round of questions. Include them only when ordering assembly or a stencil.

What drill format do Chinese fabs accept?

Excellon NC drill — usually .drl, .txt, or .xln — with metric units. Separate plated and non-plated holes when the fab asks, and keep units consistent with the Gerbers. Slots and cutouts typically go on the outline layer or as routed paths in the drill data; confirm the fab's convention first.

Should I panelize the board myself or let the fab do it?

For a standard rectangular board, letting the fab panelize is fine and usually free. Do it yourself when the shape is irregular, when fragile sections need specific depaneling treatment, or when your assembler's line has panel-size requirements. Match the V-score-versus-tabs decision to the board geometry, not to habit.

Your pre-upload checklist

Run this checklist on every export. If you cannot tick every box, fix the export before you pay — a ten-minute review beats a two-week remake.

• Design rule check passes on the final revision
• Exactly one closed board outline in the package
• All copper, solder mask, and silkscreen layers present
• Drill files complete, with plated and non-plated holes separated if the fab requires it
• Units and coordinate format consistent across every file
• Opened in a Gerber viewer: outline correct, layers aligned, drills on pads, no silkscreen on pads
• Order-form specs (thickness, copper weight, finish, mask color) match the design
• One zip archive, named for the current revision

One decision rule covers most cases: if the fab's questions keep circling the same ambiguity, the problem is in the export, not the fab. Re-export from the current design instead of patching files one by one — patched packages are how version confusion starts.

If you would rather not manage the file back-and-forth yourself, send the project to hi@cnally.com. CN Ally can check the export against the fab's requirements before you order, or vet the PCB fab itself before a production run. And if boards arrive out of spec, your exported file set is exactly what the inspection gets measured against.