Ten checks to complete before sending a PCB design for manufacture

A PCB can be electrically correct and still be difficult, expensive or impossible to manufacture as intended.

The final review therefore needs to extend beyond the schematic and layout. It must establish that the fabrication data describes one unambiguous board, that the proposed construction is within the manufacturer’s capability and that somebody other than the designer can understand what is required.

The exact limits will depend on the fabricator, material, layer count and product class. The following checks are not a substitute for the manufacturer’s own rules, but they provide a disciplined final review before the design leaves engineering.

1. Run the design rules against the intended manufacturer

A design rule check only proves compliance with the rules loaded into the CAD system. It says nothing about whether those rules match the selected process.

Confirm minimum track width and spacing, hole sizes, annular rings, copper to edge clearance, solder mask features and any rules that apply to buried or blind vias. If a manufacturer provides a rule set, use the version that matches the chosen service and stack.

Treat every waived violation as an engineering decision. A board that passes because warnings were ignored has not passed cleanly.

2. Confirm the board outline and mechanical information

The manufacturer should be able to identify one closed board outline at the correct scale. Remove duplicate outlines and construction geometry that could be mistaken for routing information.

Check the finished dimensions, cut-outs, slots, internal routing, edge plating, bevels and any areas that require controlled depth machining. Make sure the mechanical drawing and fabrication data agree.

This is also the point to confirm whether dimensions refer to finished features or tool paths. The distinction matters around routed edges and slots.

3. Freeze the layer stack and copper construction

Do not leave the fabricator to infer the intended order of copper layers, dielectric thicknesses or copper weights from file names.

Specify the layer sequence, finished board thickness, base copper, finished copper where relevant, material requirements and surface finish. If controlled impedance is required, identify the affected nets or structures and agree the stack with the manufacturer before release.

Changing the stack after layout can alter impedance, return paths, crosstalk and manufacturability. It is not merely a purchasing substitution.

4. Inspect every drill, slot and via type

Review plated and non-plated holes separately. Check finished hole sizes, tool sizes, tolerances and the relationship between holes and their pads.

Slots need particular attention because CAD tools and manufacturers do not always interpret them in the same way. Confirm whether each slot is plated, how it is represented and whether its width is compatible with the available tooling.

For blind, buried, filled or capped vias, specify the construction explicitly. A via treatment described only in an email is too easy to lose.

5. Review clearances at the board edge

Copper, pads, planes and vias close to the finished edge can be exposed or damaged during routing. Components close to the edge may also clash with panel rails, break tabs, tooling or the enclosure.

Inspect the entire perimeter, including internal cut-outs. Pay particular attention to connectors, antennas, mounting holes and intentional edge features.

If copper is meant to extend to the edge, state that requirement rather than relying on the manufacturer to recognise the intention.

6. Examine the solder mask and paste layers

Look for narrow mask slivers, openings that merge unexpectedly, covered test points and exposed copper that should be protected. Confirm how tented, filled and plugged vias are represented.

For assembled boards, review the paste apertures rather than assuming they should always reproduce the copper pads. Fine pitch devices, exposed thermal pads and small passive components may require an aperture design agreed with the assembler.

The paste layer controls deposited solder volume. It is an assembly input, not a decorative copy of the pad layout.

7. Make the legend useful and buildable

Silkscreen should identify components, polarity, pin one, test points and important warnings without printing over exposed pads or disappearing beneath components.

Check text size and line width against the manufacturer’s process. Then view the final plotted output, because automated clipping can remove the part of a reference designator that gives it meaning.

If the assembly depends on markings for orientation, confirm that they remain visible when the component is fitted.

8. Generate and inspect the actual manufacturing files

Do not approve the board by looking only at the native CAD layout. Generate the exact files that will be sent and inspect them in an independent viewer.

Check every copper, mask, paste, legend, outline and drill layer. Confirm that all layers use the same origin, scale and units. Eurocircuits identifies mismatched offsets, incorrect scaling and unnecessary files among the common causes of data problems.

Use clear filenames and include a readme or fabrication drawing that maps each file to its purpose. Remove old outputs from the release folder before creating the final archive.

9. Reconcile fabrication and assembly data

If the same supplier will assemble the board, the PCB data must agree with the bill of materials and component placement file.

Check reference designators, fitted and not fitted parts, component rotations, package names and side of board. Ensure that any panel supplied by the fabricator matches the assembler’s requirements for tooling, fiducials, rails and depanelisation.

A correct bare board is not sufficient if the assembly data describes a different design revision.

10. Freeze the release and get an independent review

Give the package a controlled revision and retain an exact copy of what was sent. Record the CAD version, output settings, approved stack, manufacturer queries and any agreed deviations.

Then ask another engineer or the manufacturing partner to review the release without relying on verbal context. If the package cannot explain itself to a second person, it is not yet ready for production.

The final question should be simple: could the manufacturer build the intended board from this package alone? If the answer depends on memory, an unrecorded conversation or a file outside the archive, the release is incomplete.

Technical references: Eurocircuits, ten rules for better production data; Eurocircuits, accepted PCB input data; KiCad PCB Editor fabrication outputs; Global Electronics Association PCB design standards.