To prepare PCB data for manufacturing, you need to supply a complete set of fabrication files that accurately represent your design intent: Gerber files for each copper layer, solder mask, and silkscreen; a drill file defining hole positions and sizes; a board outline; and a stackup specification for anything beyond a standard two-layer build. Getting these files right before you submit them is the single most effective way to avoid unnecessary delays and avoidable prototype iterations.
Incomplete or ambiguous data is one of the most common causes of manufacturing clarification cycles. A manufacturer who receives a well-prepared dataset can begin production preparation immediately; one who receives incomplete data must pause and query you, adding time and cost to your development cycle. The sections below address each element of PCB data preparation in practical detail.
What files do PCB manufacturers actually need?
PCB manufacturers need a minimum set of files that together define the physical construction of your board: Gerber files for every copper layer, solder mask layer, and silkscreen layer; a drill file specifying hole locations, sizes, and types; a board outline or mechanical layer; and a fabrication drawing or stackup specification for controlled builds. Without any one of these, a manufacturer cannot produce your board without making assumptions or requesting clarification.
The exact file list depends on your board’s complexity. A simple two-layer board requires relatively few files, while a multilayer design with controlled impedance, blind vias, or specific surface finishes requires considerably more documentation. As a baseline, prepare the following:
- Copper layers (top, bottom, and all internal layers)
- Solder mask layers (top and bottom)
- Silkscreen or legend layers (top and bottom, if used)
- Drill file or files (plated and non-plated holes separately)
- Board outline or edge-cuts layer
- Stackup specification or fabrication notes for multilayer or controlled builds
For PCB assembly, additional files are required: a Bill of Materials (BOM), a centroid or pick-and-place file, and any relevant assembly instructions. These are separate from fabrication data but equally important if you are ordering a complete manufactured and assembled board.
What is a Gerber file and what should it include?
A Gerber file is a standardised data format that describes the features on a single layer of a printed circuit board. Each file represents one physical layer of the design, such as a copper layer, solder mask, or silkscreen. Gerber files tell the manufacturer exactly where copper, mask openings, and legend markings are located on your board. The current standard is Gerber X2, which includes embedded metadata describing layer function and polarity.
Each Gerber file should include all the features relevant to that specific layer, without ambiguity. Common problems that cause manufacturing queries include:
- Missing aperture definitions or undefined macros
- Incorrect polarity settings for solder mask layers
- Copper features that extend beyond the board outline
- Solder mask openings that do not align with pad locations
- Silkscreen features that overlap pad areas, which can interfere with soldering
- Missing or inconsistent layer naming, making it unclear which file represents which layer
When exporting Gerber files from your PCB design tool, check the export settings carefully. Confirm that all layers are included, that the coordinate origin is consistent across all files, and that the file naming convention makes the layer function immediately identifiable. Using Gerber X2 format where your manufacturer supports it adds useful embedded information that reduces the risk of misinterpretation.
How should drill files be prepared for PCB manufacturing?
Drill files should be exported in Excellon format and must specify the X and Y coordinates of every hole, the finished hole diameter, and whether each hole is plated or non-plated. Plated and non-plated holes should be provided in separate files to avoid ambiguity. The drill file coordinate origin must match the origin used in your Gerber files, or hole positions will be misregistered relative to the copper layers.
Several details in drill file preparation are frequently overlooked and cause manufacturing problems:
- Finished hole size versus drill size: Specify the finished hole diameter, not the pre-plating drill diameter. Your manufacturer applies plating allowances; specifying finished size avoids double-counting.
- Separate plated and non-plated files: Mixing plated through-holes with non-plated mounting holes in a single file requires the manufacturer to interpret intent, which introduces risk.
- Via definitions: Confirm that vias are correctly defined as plated holes. Vias exported as non-plated holes will not provide electrical connection between layers.
- Blind and buried vias: If your design includes blind or buried vias, these require separate drill files for each drill stage, with clear documentation of which layers each file spans.
- Coordinate units: Confirm whether your drill file uses metric or imperial units, and that this matches the format your manufacturer expects.
After export, visually verify your drill file against your Gerber copper layers using a PCB data viewer. Misregistered holes are difficult to detect by reviewing raw file content but immediately visible when layers are overlaid.
What design rules should be checked before sending PCB data?
Before submitting data for manufacturing, your design should be checked against the manufacturing capabilities of your chosen process. The most important design rules to verify include minimum track width and spacing, minimum annular ring on drilled holes, copper-to-board-edge clearance, minimum drill size, solder mask expansion, and any impedance or stackup constraints. Violations of these rules are the most common cause of avoidable manufacturing problems.
Running a Design Rule Check (DRC) within your PCB design tool is a necessary first step, but it only checks against the rules you have configured. If those rules do not accurately reflect your manufacturer’s capabilities, the DRC will pass designs that cannot actually be manufactured. Always obtain and apply your manufacturer’s specific design rules rather than relying on generic tool defaults.
Key areas to review before submission include:
- Track width and clearance: Minimum values depend on the PCB technology and the manufacturing process selected. Standard pooled production has different limits from fine-line or HDI processes.
- Annular ring: The copper ring remaining around a drilled hole must meet the manufacturer’s minimum. Undersized annular rings risk drill breakout and open connections.
- Copper-to-edge clearance: Copper features that are too close to the board edge can be damaged during routing. A minimum clearance is required for reliable production.
- Solder mask slivers: Very narrow strips of solder mask between adjacent pads can lift or collapse during processing. Check that mask openings do not create unsupported slivers.
- Drill-to-copper clearance: Non-plated holes and slots that are too close to copper features can cause shorts or damage during drilling.
A DFM analysis performed before submission identifies these issues while changes are still straightforward. Identifying a track spacing violation after a prototype has been produced means a redesign, a new order, and additional lead time. Identifying it before submission costs nothing beyond the time to correct the file.
What information should a PCB stackup specification include?
A PCB stackup specification should define the number of layers, the layer order, the dielectric materials and thicknesses, the copper weights for each layer, the required finished board thickness, and any controlled impedance requirements. For standard two-layer builds, many manufacturers use predefined constructions, but for multilayer, controlled impedance, or high-frequency designs, a complete stackup specification is essential to ensure the board is built to your electrical and mechanical requirements.
Without a clear stackup specification, a manufacturer must make assumptions about construction. Those assumptions may not match your design intent, particularly if your design relies on specific impedance values, dielectric properties, or layer thicknesses for signal integrity.
A complete stackup specification for a controlled build should include:
- Total number of layers and their sequence (signal, plane, mixed)
- Copper weight for each layer (typically expressed in grams per square metre or ounces per square foot)
- Dielectric material type and thickness for each layer pair
- Target finished board thickness and acceptable tolerance
- Controlled impedance requirements, including target impedance values, the relevant layers, and the trace geometry used for calculation
- Surface finish specification (for example, ENIG, HASL, OSP)
For manufacturers who offer predefined stackup constructions, selecting from an approved build is often more efficient than specifying a fully custom stackup. Predefined builds have been validated for manufacturability, which reduces the risk of stackup-related problems during production.
How does an online PCB data verification tool help before ordering?
An online PCB data verification tool analyses your design files against manufacturing rules before you place an order, identifying potential problems while changes can still be made digitally. This is more useful than receiving a query from a manufacturer after submission, because you can correct issues immediately without waiting for a manufacturing review cycle. Verification tools can check data completeness, flag DFM violations, and show you how your design will be interpreted for production.
The practical value of pre-submission verification is that it separates avoidable manufacturing problems from genuine engineering development. Engineering iterations are a normal and necessary part of prototype development. Iterations caused by incomplete data, misinterpreted layers, or overlooked design rule violations are not necessary and add cost and time without advancing your design.
A capable verification tool does more than flag errors. It visualises your manufacturing data so you can confirm that your copper layers, drill positions, solder mask openings, and board outline are all correctly interpreted. This is particularly important when working with a new design tool, a new export configuration, or an unfamiliar PCB technology.
How Eurocircuits PCB Visualizer helps with PCB data preparation
Eurocircuits‘ PCB Visualizer is a free online engineering environment that connects your design data directly to the manufacturing process. It is designed specifically to support the kind of pre-submission verification described throughout this article. Key capabilities include:
- Automated data integrity checks to confirm that all required files are present and correctly formed
- Over 700 DRC and DFM rules applied against the selected pooling service, identifying manufacturability issues before production begins
- A visual digital twin of your design showing how each layer will be interpreted for manufacturing
- An integrated stackup editor with over 970 predefined builds for controlled impedance and multilayer designs
- Automatic repair suggestions for identified issues, allowing you to review and approve corrections without leaving the platform
- Access to a verified component database of 450,000 parts to support assembly preparation
The Visualizer is available 24 hours a day, seven days a week, in six languages, and is integrated directly into the Eurocircuits ordering workflow. Engineers can verify their data, review the manufacturing interpretation, and place an order within a single session. If you are preparing PCB data for manufacturing and want to identify avoidable problems before committing to production, upload your design to PCB Visualizer and review the results before you order.