Key Takeaways
- Never generate manufacturing archives manually via File -> Fabrication Outputs -> Gerbers; use a version-controlled OutputJob (.OutJob) file for 100% deterministic exports.
- Standardize on 2:5 format (or 4:5 metric) in Altium's Gerber Setup to prevent coordinate rounding errors on 0.4mm and 0.35mm ultra-fine pitch BGA escape routings.
- Ensure that Gerber Output Origin and NC Drill Origin match exactly (both set to Absolute Origin or Relative Origin) to prevent drill holes drifting off copper pads.
- Explicitly map Mechanical 1 (or Board Shape) to all Gerber layer setups, or export a dedicated Route/Milling layer for internal cutouts and slots.
1. Why Professional Workflows Require OutputJob (.OutJob) Files
In Altium Designer, engineers can generate manufacturing data either manually through the interactive PCB Editor menus (File -> Fabrication Outputs) or automatically using Output Job configuration files (*.OutJob). Relying on manual menu clicks is an anti-pattern in professional hardware engineering: manual exports frequently lead to forgotten drill files, mismatched coordinate origins, or omitted solder mask layers.
An OutputJob document acts as an immutable, version-controlled recipe for all production deliverables. It encapsulates exact Gerber layer selections, aperture configurations, drill parameters, pick-and-place files, and assembly drawings into unified output containers.
By standardizing an OutJob template across your engineering organization, any engineer can generate 100% bit-for-bit identical manufacturing archives with a single click, eliminating human error from the release cycle.
Store your production .OutJob template in your company's global Altium Workspace or Git repository. When starting a new PCB design, import this verified configuration rather than manually setting up Gerber parameters.
2. Gerber Setup: 2:4 vs 2:5 Precision and Units
When configuring the Gerber Output generator inside an OutJob file, the first critical dialog is the Gerber Setup window. In the General tab, you must define the Units (Inches vs Millimeters) and the Format (coordinate integer and decimal precision).
Historically, the 2:4 format (2 integer digits, 4 decimal digits in inches) was the industry standard. In 2:4 format, the smallest addressable increment is 0.0001 inches (0.1 mil or 2.54 µm). While sufficient for coarse through-hole boards, modern high-density interconnect (HDI) designs feature 0.4mm pitch BGAs, 3 mil trace/space geometries, and micro-vias. Truncating coordinates to 0.1 mil introduces cumulative rounding errors that cause subtle polygon distortions and aperture snapping artifacts.
Always configure your Gerber Setup to 2:5 format (Inches) or 4:5 format (Millimeters). In 2:5 format, the coordinate resolution improves by an order of magnitude to 0.01 mil (0.254 µm or 254 nm), easily resolving nanoscale EDA vector geometries without coordinate degradation.
Always select 'Suppress leading zeros' and 'Absolute origin'. Using 'Suppress trailing zeros' is an archaic standard that causes coordinate parsing errors in modern automated CAM ingestion engines.
%FSLAX25Y25*%
%MOIN*%
%ADD10C,0.00800*%
%ADD11R,0.04000X0.02000*%
D10*
X0125430Y0345210D02*
X0125430Y0350210D01*3. NC Drill Setup: Preventing Origin Offset Mismatches
The most catastrophic mistake in Altium CAM generation occurs when the Gerber and NC Drill outputs use conflicting coordinate reference origins. In Altium's Gerber Setup, the Origin setting defaults to 'Absolute Origin'. However, in the NC Drill Setup dialog, engineers often mistakenly select 'Relative Origin'.
When this occurs, the copper layers are plotted relative to the absolute sheet coordinate (0,0), while the drill holes are plotted relative to the PCB's user-defined relative origin (e.g., the bottom-left corner of the board outline). The resulting files appear completely misaligned: the drill holes appear miles away from the copper pads when loaded into a CAM viewer.
To ensure flawless layer registration:
1. In Gerber Setup -> Advanced: Set Origin to 'Absolute Origin'.
2. In NC Drill Setup: Match Units (Inches) and Format (2:5) to the Gerber Setup, and set Origin to 'Absolute Origin'.
3. Check 'Generate separate files for plated/unplated holes' to produce both .TXT (plated) and -NonPlated.TXT drill files.
| Altium Drill File Extension | Drill Type | Plating Requirement | Manufacturing Step |
|---|---|---|---|
| .TXT (or .DRL) | Plated Holes (PTH) | Electroless + Electroplated Copper | Drilled before outer copper plating |
| -NonPlated.TXT | Unplated Holes (NPTH) | Raw Dielectric / Bare FR-4 | Drilled after outer copper plating |
| .LDP | Layer Pairs Descriptor | Metadata / Layer Pairing Info | Used by CAM to verify drill layer spans |
| .DRR | Drill Report | Text Documentation | Human-readable tool size summary table |
4. Mechanical Layer Traps: Board Outline, Slots, and Routing
In Altium Designer, mechanical layers are fully customizable, leading to widespread ambiguity across engineering teams. Some designers place board outlines on Mechanical 1, others on Mechanical 3, Mechanical 15, or the specialized Keep-Out Layer.
Fabricator CAM operators do not know which mechanical layer represents your intended board contour unless it is explicitly exported and named. Crucially, the 'Keep-Out Layer' in Altium is an internal EDA clearance barrier, NOT a manufacturing outline. Never export the Keep-Out layer as your sole board contour.
Best Practice: Designate Mechanical 1 (or Board Shape) as your official Board Outline layer. In your OutJob Gerber configuration, map Mechanical 1 to a dedicated Gerber layer file (typically yielding a .GM1 or .GML extension). For boards containing internal mill-out slots, routed cutouts, or plated edge castellations, export a dedicated NC Route file (.RNC) or Route Tool Path layer.
5. Packaging Verified Fabrication Archives & Pre-Flight Audit
Before releasing your Altium manufacturing ZIP to procurement or uploading to a CAM web portal, execute this mandatory verification protocol:
- Validate OutJob Containers: Execute the 'Fabrication Outputs' batch container to generate all artwork and drill files into your clean output folder.
- Confirm File Count: Verify the presence of all copper layers (.GTL, .GBL, .G1, etc.), solder masks (.GTS, .GBS), silkscreens (.GTO, .GBO), board outline (.GML / .GM1), and drill files (.TXT).
- Assemble Fabrication ZIP: Compress all generated CAM deliverables into a single release archive named [Project]_[Revision]_FAB.zip.
- Load Archive into GerberPatch: Open GerberPatch in your browser and drag the ZIP archive directly into the viewer.
- Audit Coordinate Registration: Verify that NC Drill hole centers land concentrically on through-hole via pads across all copper layers.
- Inspect Board Contour: Ensure the board perimeter is rendered as a clean, single-pixel boundary line without missing edge segments or stray mechanical text.
Inspect your Gerber files 100% privately
Verify clearances, layers, and drill holes with zero cloud uploads in GerberPatch.