GlobalWellPCBPCB & PCBA Manufacturing
GlobalWellPCB

PCB Fabrication File Requirements

Define geometry, construction and release authority before fabrication.

Review the requirementsDownload templates
Manufacturing handoffIllustrative package
GBRCopper_L1.gbr
DRLPTH_and_NPTH/
PDFStackup_and_Fab_Drawing.pdf
TXTRelease_Manifest.txt

One consistent file set, with a clear revision.
Include any questions for your project contact.

01
Define the releaseRevision & configuration
02
Check the dataGeometry & conventions
03
Prepare the handoffProject files and questions

Build a complete bare-board handoff

Prepare machine-readable geometry, a clear construction specification and one controlled release.

A fabrication package must describe both the board geometry and the required construction. Gerber carries layer imagery and attributes; a Gerber Job file can also carry manufacturing characteristics such as thickness and finish. Check what your export actually contains.

Practical file-preparation checklist — confirm the receiving fabricator’s intake requirements
DeliverableWhat to prepareReview before releaseTypical representation
Layer artworkCopper layers, mask and legend where specifiedIdentify layer function and top-to-bottom order; omit unrelated sketches.Gerber RS-274X / X2, or an agreed integrated dataset
Board profileClosed board boundary and internal cutoutsUse one governing outline; add dimensions and tolerances in the drawing.Dedicated profile data + dimensioned drawing
Drill / route dataHole tools, locations, slots and relevant depth/span informationDistinguish plated and non-plated features; identify blind/buried spans.Documented NC drill / route, or agreed equivalent
ConstructionMaterial, stackup, finished thickness and copper requirementsState exact requirements and any permitted substitutions.Fabrication drawing / stackup / populated job data
Special requirementsImpedance, via treatment, special finishes and panel detailsIdentify applicable layers, locations, tolerances and approvals.Referenced tables and dedicated process drawings
VerificationAcceptance criteria, required tests and reportsSpecify what is required, not only “standard testing.”Order requirements; design netlist where requested
Release identificationProject, revision, release purpose and quantity basisReconcile filenames, drawings and dataset before sending.Release manifest

Make holes, slots and the outline unambiguous

Explicit classification is safer than asking the receiver to infer your intent.

  1. 01

    Classify every hole type

    List PTH and NPTH explicitly. Name the start and stop layers for non-through features. A copper pad around a hole is not a reliable instruction for whether it should be plated.

  2. 02

    Provide machining data, not only a drill map

    A drill map is a visual check. Supply the actual accepted NC data or integrated dataset, with tools, units and coordinate interpretation. Explain slots and routing separately where needed.

  3. 03

    Specify finished requirements

    State finished hole or slot dimensions and tolerances. Let the fabricator define compensated tool sizes unless a particular tooling requirement has been agreed.

  4. 04

    Overlay the output

    Compare holes, pads and the governing profile in a CAM viewer. Check a known board dimension, cutout location and a reference hole before release.

Write the construction requirements once

Stackup and material

Identify layer count, layer order, material grade, dielectric construction and finished board thickness. Where dielectric thickness is critical, distinguish the pressed construction from an unpressed material designation.

Copper and finish

Distinguish starting foil from required finished copper. Identify surface finish, selective areas, mask and legend requirements. Avoid leaving “1 oz” as the only description of a plated outer layer.

Impedance and change authority

Provide net group, signal layer, reference layer(s), target and tolerance. State which widths, gaps or materials can be adjusted only after your approval.

Special construction

For flex, rigid-flex, blind vias, backdrill, edge plating, filled vias or selective processes, supply location-specific drawings and review the process with engineering before release.

Package the release for review

One design revision, one file map and no unexplained competing outputs.

Controller_RevB_RFQ/
  00_Release_Manifest.txt
  01_Fabrication/
    Copper_*.gbr
    Mask_*.gbr
    Profile.gbr
    Drills_PTH.drl
    Drills_NPTH.drl
    Stackup_and_Fab_Drawing.pdf
  02_Verification/
    Design_Netlist.ipc
    Impedance_Requirements.csv

This folder tree is an organizational example, not a required upload structure. Some intake systems require a flat archive. Preserve the internal structure of an ODB++ dataset; do not flatten it to resemble a Gerber upload.

Extensions are illustrative. Altium, for example, can output ASCII drill data as .TXT; its .DRL output can be binary. Inspect the export type, not just the filename.

An IPC-D-356 design netlist can support bare-board manufacturing checks. It is not a replacement for layer artwork or a complete fabrication dataset.

Download the preparation files

Download the checklists and templates below without signing in or submitting a form.

Fabrication specification worksheet

Blank construction, drill, finish, impedance and acceptance requirements.

TXT · 1.3 KB
Download

Release & coordinate manifest

Identify the file revision, stackup and coordinate conventions, and list any details you need help confirming.

TXT · 2.8 KB
Download

Read before using the templates

Field definitions, limitations and release-control notes.

TXT · 3.5 KB
Download

Frequently asked questions

Are Gerber files alone enough?

Not necessarily. Check that the package includes the required drill/route information, profile and manufacturing specification. A populated integrated dataset or Gerber Job file may carry some requirements, but missing fields still need to be supplied.

Do you always need separate PTH and NPTH files?

You need an unambiguous distinction. Separate files are one practical method; an agreed format with explicit attributes is another. Confirm the receiver’s preferred representation.

Is a PDF fabrication drawing a substitute for machine data?

Treat it as supporting documentation unless a specific engineering conversion service has been agreed. Do not assume an ordinary plotted PDF contains a complete, machine-ready board definition.

Should a design netlist be extracted from the exported Gerbers?

For an independent connectivity comparison, supply the released design netlist when requested. A netlist reconstructed only from the same exported geometry cannot independently prove that the export matches the original design intent.

Does completing this checklist authorize production?

No. It prepares the handoff. Engineering acceptance, approved changes, commercial terms and the final release decision remain separate.

Technical references & scope

  1. [1] Ucamco — Official Gerber format overview
  2. [2] Ucamco — Gerber Job file
  3. [4] KiCad 10.0 — PCB Editor: manufacturing outputs
  4. [5] Altium Designer — Preparing fabrication data

Use the checklists and templates on this page to prepare your manufacturing files. Confirm the required formats and approved design revision with your project contact before ordering; export steps may vary by CAD software.

GlobalWellPCB

File preparation resources for PCB & PCBA projects.

Back to top
Scroll to Top