Gerber data preparation is the controlled release process that converts a PCB design into a synchronized, reviewable manufacturing package. It includes the plotted images, drill and route data, fabrication drawings, stackup, net intent, revision identity, assembly outputs, and acceptance requirements needed to build the intended board. It is not merely a ZIP folder of copper layers exported without verification.
A syntactically valid Gerber file can still describe the wrong revision, omit non-plated slots, conflict with the fabrication drawing, or align perfectly with an outdated drill file. This guide outlines the stringent requirements for creating a foolproof Gerber release package to prevent manufacturing delays and field failures.
The Core Dataset: What Information Does Gerber Carry?
Gerber (RS-274X) describes precise two-dimensional images used in PCB fabrication, including copper, solder mask, legend, paste, and—in supported workflows—drill data. Extended Gerber embeds apertures directly in the file, eliminating the need for a separate aperture wheel.
Gerber X2 preserves the image model and adds standardized attributes. These attributes identify a file's function (e.g., top copper vs. bottom mask), distinguish features such as SMD pads and vias, and carry component, pin, or net information. A .gbrjob Gerber Job File often accompanies the images, providing machine-readable board information such as layer structure and selected fabrication characteristics.
However, attributes reduce manual interpretation but do not authorize silent assumptions. The receiving CAM (Computer-Aided Manufacturing) engineer still requires the controlled revision, construction and finish details, tolerances, special processes, IPC acceptance class, and test deliverables.
Format Comparison: Gerber X2 vs. ODB++ vs. IPC-2581
Use a format both you and your manufacturer can generate, import, compare, archive, and return without losing meaning. Richer data is not safer if downstream tools strip it or misinterpret it.
| Format | Practical Strength | Release Consideration |
|---|---|---|
| Extended Gerber (RS-274X) | Broad tool and factory support; highly transparent image files. | Layer function, stackup, net intent, and assembly data rely heavily on companion files (drawings, netlists). |
Gerber X2 + .gbrjob |
Adds standardized image attributes and machine-readable job information while retaining Gerber images. | Confirm that the receiving CAM flow supports the attributes actually exported by your EDA tool. |
| ODB++Design | Structured PCB product model that transfers design and manufacturing information in one comprehensive dataset. | Confirm version compatibility, import results, and the manufacturer's return-data policy. |
| IPC-2581 / IPC-DPMX | Open, bidirectional PCB design and manufacturing description standard. | Agree upon the revision, content level, supported features, and validation workflow prior to release. |
Building a Controlled Release Manifest
A release manifest prevents mixed revisions. Put it inside the release archive and align it precisely with the purchase order and fabrication drawing title block.
Release Manifest Checklist
A robust manifest must explicitly define the boundaries of the released dataset.
- Product Identity: Part number, board name, revision, variant, and customer name.
- Source Identity: CAD tool/version and source project revision or Git commit hash.
- File Inventory: Filename, purpose, layer/function, and units (Imperial/Metric).
- Integrity Record: SHA-256 checksum for each file or the final archive to detect corruption.
- Applicable Documents: Explicit revisions for the fabrication drawing, stackup, impedance table, material spec, and assembly requirements.
- Supersession Note: Explicitly state which prior package is obsolete to prevent prototypes from returning in mass production.
Preflight Verification: Inspecting the Exported Data
Open the final exported archive in an independent Gerber/CAM viewer before sending it to the manufacturer. Reviewing only the PCB editor proves the design is correct in the EDA tool, not that the release package was generated correctly.
1. Geometric and Visual Review
- Confirm layer count, order, registration, orientation, dimensions, origin, and profile closure.
- Verify top-side text reads correctly (Right-Reading) and bottom-side text follows the agreed viewing convention.
- Inspect copper-to-profile clearances, internal cutouts, slots, castellations, edge plating, and V-scoring lines.
- Compare Plated Through-Hole (PTH) and Non-Plated Through-Hole (NPTH) locations with pads and mechanical drawings.
- Inspect solder mask openings, mask dams, tented/plugged vias, and exposed-copper features.
2. Semantic and Cross-File Review
- Reconcile drill spans with the approved stackup (especially for blind/buried vias).
- Compare the IPC-D-356 netlist against the Gerber copper traces.
- Match assembly references across the BOM, Centroid (Pick & Place) file, and assembly drawings.
Resolving Conflicts: The Designer vs. Manufacturer Boundary
Files within a release package can each be syntactically valid while disagreeing with one another. When a manufacturer identifies a conflict, they will issue an Engineering Query (EQ). The manufacturer must never guess the designer's intent.
| Conflict Type | Manufacturer's Responsibility | Designer's Responsibility |
|---|---|---|
| Gerber Profile vs. Drawing Dimension | Halt CAM and issue an EQ. Do not scale or assume which datum is correct. | Provide a customer-approved dimensioned profile or upload a corrected Gerber package. |
| Stackup Drawing vs. Gerber Job File | Report the mismatch. Do not substitute dielectrics without authorization, as it changes impedance. | Provide the approved stackup revision and regenerate the .gbrjob metadata. |
| Drill File vs. Pad Geometry | Identify tool size mismatches or ambiguous plated status (PTH/NPTH). | Supply an updated hole table alongside corrected drill/pad data. |
| Solder Mask Image vs. Via-Fill Note | Flag the discrepancy. Tenting, plugging, filling, and capping are distinct processes. | Define the exact feature-level via treatment and the required acceptance standard. |
| Impedance Table vs. Routed Geometry | Calculate the required trace width for the target impedance based on actual materials and issue a proposal. | Review the supplier's field-solver results and explicitly approve the stackup proposal. |
Controlling CAM Edits and Manufacturing Compensation
PCB fabrication requires process compensation and tooling. The supplier will adjust working data to achieve the released finished result (e.g., etch compensation), but they must not reinterpret product function.
- Routine Compensation (No Approval Required): Etch, plating, imaging, or drill compensation within qualified process planning to meet contractual tolerances.
- Supplier Panelization (Shared/Approved): Adding panel rails, tooling holes, fiducials, coupons, or thieving outside the customer profile.
- Design Intent Changes (Requires Written Approval): Modifying annular rings, copper trace routing, padstacks, spacing, net connectivity, hole types, or the board outline. Substituting stackup material (e.g., swapping a high-speed dielectric) also requires explicit requalification.
Conclusion
Reliable Gerber data preparation is a strict release-control discipline. Generating one synchronized package, identifying it with a manifest and checksums, independently inspecting its images and semantics, closing conflicts through EQs, and approving the supplier's CAM interpretation before production prevents manufacturing disasters. This rigorous workflow mitigates far more risk than relying on a generic "DFM Passed" check.
After the file package is ready, use the HilPCB capabilities overview to select the appropriate fabrication, assembly, testing, or integration route.
Frequently Asked Questions
What is the minimum Gerber package for PCB fabrication?
At minimum, provide every copper, solder mask, legend, and required mechanical layer; plated and non-plated drill/route data; a clear board profile; and fabrication requirements (drawing/notes). Multilayer, impedance-controlled, HDI, or special-process boards also require an approved stackup, via definitions, material details, and test requirements.
Is Gerber X2 better than standard Gerber (RS-274X)?
Gerber X2 adds standardized attributes that reduce ambiguity and can carry net and feature information. It is preferable when both the EDA tool and the manufacturer's CAM flow support it. However, correct revision control, companion documents, and independent viewing remain strictly necessary.
Can a PCB manufacturer change Gerber data during CAM preparation?
The manufacturer normally creates compensated working data (e.g., etch compensation) to achieve the specified finished board dimensions. However, changes to connectivity, padstacks, trace spacing, board outline, hole types, or base materials alter the design intent and strictly require written engineering approval.
Does a "DFM Pass" guarantee high manufacturing yield?
No. DFM reduces identified manufacturability risks for a stated process, but yield also depends on design maturity, process capability, materials, measurement systems, assembly, test, and change control. Always request the DFM scope and actual supplier evidence rather than a generic pass/fail badge.