1.3 CAD/CAM Outputs: Fabrication Package Definition

The fabrication package is the blueprint for the physical substrate. If this data is incomplete, the PCB fabricator (CAM engineer) will fill in the gaps with assumptions. Assumptions in manufacturing are the root cause of "silent failures"—boards that pass continuity testing but fail in the field due to incorrect impedance or material selection.

Define "Fab-Ready" as a dataset that requires zero engineering questions (EQs) to interpret. The goal is to move from "CAM Interpretation" to "CAM Execution."

The Primary Data Format

Select one format and enforce it. Do not mix formats within a single release.

Option A: Intelligent Formats (Recommended)

Use ODB++ (.tgz) or IPC-2581 (.xml).

• Why: These are single-file containers that include netlists, stackups, and drill data in a structured hierarchy. They eliminate the risk of missing layers or misaligned drill files.
• IPC-2581 Note: This XML-based standard allows bi-directional data exchange and explicitly defines stackup materials, preventing the "PDF vs. Gerber" conflict.

Option B: Legacy Gerbers (RS-274X / X2)

If you must use Gerbers, you must bundle the following explicitly. A loose collection of .gbr files is not a fabrication package.

1. Gerber Files: All copper, mask, silk, and paste layers.
2. NC Drill File: Excellon format. Must specify units (English/Metric) and coordinate suppression (Leading/Trailing zeros).
3. IPC-D-356 Netlist: Required for bare-board electrical test (BBET). Without this, the fab only checks if the board matches the Gerbers, not if the Gerbers match the schematic.

Essential Fabrication Elements

To prevent "silent assumptions," the following elements must be explicitly defined in the data pack.

1. The Board Outline & Profile

Do not rely on the copper pour to define the board edge.

• Requirement: dedicated "Mechanical" or "Profile" layer containing a continuous, closed zero-width line.
• Logic: If the outline is open or duplicated on multiple layers ⭢ Then the router path is undefined, risking board dimensions.

2. Drill Definitions

Ambiguous drill charts cause hole-size violations.

• Separation: Separate Plated Through Holes (PTH) from Non-Plated Holes (NPTH) in the drill file headers.
• Tolerance: Define tolerance per hole type (e.g., Press-fit connectors require tighter tolerance than standard vias).
• Slot/Route: Define slots in the specific Drill_Plated or Route layer, not just on the board outline layer.

3. Stackup & Impedance Table

Never bury stackup requirements in an email. Embed them in the fabrication drawing or the ODB++/IPC-2581 metadata.

• Material: Specify the IPC-4101 slash sheet (e.g., "/126" for High Tg FR-4), not a brand name (e.g., "Isola 370HR"). Brand names lock the supply chain; IPC specs allow equivalent substitutions.
• Impedance: List the target impedance (e.g., 50Ω SE), the reference layer, and the trace width required to achieve it.
• Logic: If impedance is critical ⭢ Then add a "Test Coupon" requirement to the fabrication notes.

The Fabrication Drawing

The Fab Drawing is the contract. If a requirement is not here, the fabricator is not liable for missing it.

Mandatory Notes:

• Class: IPC-6012 Class 2 (Standard) or Class 3 (High Reliability).
• Finish: ENIG, HASL, Immersion Silver, etc. (Specify thickness if critical).
• Color: Solder mask and Silkscreen color.
• Standards: "Workmanship shall conform to IPC-A-600."

Pro-Tip: Add a "Do Not X-Out" note if your pick-and-place machines cannot handle panelized boards with bad units. Otherwise, fabs will deliver panels with rejected boards crossed out with marker.

The Netlist Compare Rule

The most critical safety net in PCB fabrication is the Netlist Compare.

The Process:

1. Output: Generate IPC-D-356 netlist from CAD.
2. Intake: Fab CAM extracts a netlist from the Gerbers/ODB++.
3. Compare: The CAM system compares CAD Netlist vs. Gerber Netlist.

Logic ⭢ Action:

• If short/open is detected ⭢ Stop. This indicates the Gerbers do not match the electrical design (schematic).
• Mandate: Explicitly state in the Fab Drawing: "Electrical Test 100% required against IPC-D-356 Netlist."

Final Checklist

Check	Requirement	Pass Metric
Data Format	ODB++ / IPC-2581 / Gerber+Drill.	Single archive, valid checksum.
Netlist	IPC-D-356 included.	Matches CAD database.
Outline	Closed, single contour.	Mechanical layer clear of debris.
Stackup	Defined in drawing or file metadata.	Dielectric thickness & copper weight explicit.
Drills	PTH/NPTH separation.	Drill chart matches tool sizes.
Fab Notes	Material, Class, Finish defined.	No "TBD" values in notes.