Displayed Gerber graphics establish only that geometry was read, not that the factory knows every layer function, hole type, and manufacturing condition. Map copper, mask, legend, outline, and drilling explicitly, freezing them with materials, stackup, and revision notes. Extensions assist identification but do not replace attributes/lists.
Graphics, attributes, and manufacturing notes have different roles
Ucamco describes Gerber layer files for copper, mask, legend, and drill/rout data; attributes describe layer/object semantics, while Gerber Job adds thickness, materials, finishes, and other characteristics. A line alone may not identify outline, annotation, or machining path; missing semantics require explicit lists.
| Content | Primary Expression | Delivery Inspection |
|---|---|---|
| Copper graphic | Geometry and related attributes of each conductive layer | Layer number, layer function, polarity, and connection |
| Solder Mask and Text | Windows, coverage, and characters | Side, direction, and relationship to pads |
| Holes and Slots | Via locations, shapes, plated hole attributes, and layer pairs | PTH/NPTH, start/end layers, and coordinates |
| Non-Graphic Requirements | Material, thickness, processing, and special processes | Consistency among manufacturing drawings, Job files, and notes |
Exporter attribute support varies; selecting “X2” does not establish completeness. Inspect exported files and confirm what the receiver can actually read.
How to write file mapping for six-layer board
An engineering example labels six copper layers L1 through L6, separately listing Top/Bottom mask, Top/Bottom legend, outline, PTH, and NPTH. Include design layer names, such as continuous ground reference for L2, to avoid alphabetical stacking. List L1-to-L2 blind vias separately from L1-to-L6 through-holes; do not combine them in an unidentified file.
- List actual filenames, functions, sides/layers, and current-revision status individually.
- Match copper-layer count to stackup; investigate missing layers or additional obsolete layers.
- Map drilling to correct layer pairs, distinguishing round holes, slots, and milling data.
- Specify one closed outline, defining internal cutouts and panel boundaries.
- Link manufacturing conditions unavailable from graphics to same-revision notes.
The example organizes information without prescribing extensions. Automated identification and manual lists must identify the same objects.
Independently check units, origins, and mirroring
Unit errors often scale all dimensions by a fixed ratio. If a 50 mm board edge appears as 1.9685 mm, inch/millimeter interpretation may be involved: 50÷25.4≈1.9685 helps locate the issue, but inspect actual unit declarations too. Do not merely adjust display zoom until it looks close.
Use consistent origins/orientations for copper, drills, and outline. Flipping the display differs from mirrored export; viewing the bottom does not authorize additional mirroring. Check asymmetric holes, locating notches, and text together; a symmetric rectangle may conceal reversal.
| Inspection Items | Selectable reference | Error Indicators |
|---|---|---|
| Dimension | Known outline length and width or hole pitch | All adjusted by multiples of 25.4 deviation |
| Origin | Alignment Holes and Copper Pads | Hole and all pad overall offset |
| Orientation | Asymmetric notch and text | Bottom layer or hole group left-right reversal |
| Polarity | Large copper areas and isolation zones | Plane copper and blank area swap |
Check both electrical and mechanical hole functions
Plated holes' connected layers, finished diameters, and hole-wall copper differ from nonplated mounting holes. Define slot shapes, machining, and plating too. Cross-check hole-table counts/diameters against actual files to prevent obsolete tables mixing with new geometry. Blind/buried vias need layer pairs/structures; factories must not infer them from pad locations.
Overlay holes, copper, and mask to check target-pad alignment, mounting-hole copper clearance, and slot/edge intersections. Calculated nominal annular rings do not replace fabricated residual-ring criteria. Specify special filling/capping separately by hole group.
From independent viewer to netlist cross-check
Open files from the final archive in an independent viewer, not only the CAD design. Check layers, dimensions, orientation, and hole groups first, then fine pitch, plane isolation, mask, and outline relationships. Match any supplied netlist to layout revision for receiver connectivity cross-checking; netlist presence does not establish use, so retain check records.
Visual inspection finds wrong layers/offsets but not all connections. Netlists, graphics, and notes also serve different purposes. Record tool/version, reviewed objects, findings, and closure, beyond “Gerber normal.”
Re-freeze entire package after finding issues
For wrong layer names, outlines, or drills, revise the design/export settings and regenerate the complete package. Avoid manual Gerber changes without source updates. Approve manufacturing compensation jointly and retain before/after files and purpose instead of silently overwriting geometry.
Release lists should identify package revision, generation time, file count, and checksum, removing obsolete remnants from the current package. Checksums establish content identity, not engineering correctness. After clarifications close, everyone should reference one package instead of combining chat attachments into multiple final versions.
For first deliveries, confirm the receiver identifies layers/attributes as intended. Supplement unsupported attributes with controlled lists and retain feedback. Compatibility need not remove useful semantics; ensure both representations agree.
Link viewer projects to the final package too. Remembered manual alignment/colors may hide original-file issues on reopening. Recheck critical coordinates in a clean import and document required receiver mappings. Export and inspection are separate actions; one CAD screenshot cannot replace both.
Avoid misinterpretation when checking planes and attributes
For large copper planes, confirm polarity, clearances, and thermal connections match the design. A complete rectangular display does not establish correct internal clearances. Overlay connected pads, unconnected holes, and edges, checking attributes against the layer list. For negative planes especially, blank display does not mean absent copper.
If outlines and dimension annotations are exported together, receivers may struggle to identify the machining path. Separate the unique outline, internal cutouts, and explanatory drawings, checking known dimensions. Investigate duplicate, unclosed, and stray distant geometry so annotations are not milled.
Attributes provide semantics but do not excuse geometry checks. A copper-tagged file may be obsolete; a through-hole-tagged file may have wrong layer pairs. Cross-check attributes, lists, and graphics to expose inconsistencies faster than any alone.
Record findings by file, object, and location with the corresponding source-design item. This enables source/export correction rather than untraceable receiver-side repairs. Confirm successful import separately from correct engineering definitions.
Frequently Asked Questions
Can PDF manufacturing drawings replace Gerber?
Drawings explain requirements and generally cannot replace precise graphics and hole data.
Can production start once opened?
Complete semantics and manufacturing review are still needed. Continue to Gerber Job consistency, Manufacturing Combination and Delivery List.
Source material and applicable scope
- Ucamco, “Gerber Format — Official Gerber Format Website”; official overview webpage, not the full format specification; checked on 2026-10-17; relevant sections: Gerber layer-file, attribute, and Job-file responsibilities. Supports graphics/semantic roles. Checklists and configuration examples are engineering guidance, not complete syntax coverage.
