PCB design review: a checklist before you order prototype boards

Boards are cheap to change in CAD and expensive to change after they ship. Here is how we review a schematic, a layout, and the fab package before a prototype order, and where AI review tools fit.

November 11, 20269 min read

Written by Konstantin Dolgan, Ph.D., NPDP

Founder & CEO, Product Development Engineer

Published November 11, 2026

What is a PCB design review?

A PCB design review is a planned check of a circuit board design by someone other than the person who drew it, done before the board is released for fabrication. It covers three things: whether the schematic does what the product needs, whether the layout can be built and will behave, and whether the files you send to the fab and assembly house describe the board you think you designed.

For a prototype, the review is not a formality. A missed footprint error or a swapped pin can turn a board order into a rework session or a full respin. The review is where you catch those problems for the price of an afternoon instead of a new lot of boards.

When to run a PCB review in a prototype program

Run a short review at each point where the design is about to get harder to change. In our programs that usually means three passes:

Pass	When	Main question	Typical inputs
Schematic review	Before layout starts	Will this circuit work and can we buy the parts?	Schematic PDF, block diagram, requirements, BOM draft, key datasheets
Layout review	Placement done, then again after routing	Will this board fit, behave, and be testable?	Layout files, stackup, mechanical outline / enclosure CAD, placement notes
Release review	Right before ordering	Are the fab and assembly files complete and consistent?	Gerbers or ODB++, drill files, pick and place, BOM with manufacturer part numbers, fab and assembly notes

The placement check matters more than people expect. Connector positions, mounting holes, and tall parts are tied to the enclosure. Catching a clash at placement is a quick move; catching it after routing can mean rerouting a large part of the board. That is also why the layout review should include whoever owns the mechanical design (see our guide to enclosure design for electronics).

Schematic review: what to check

A schematic review checks that the circuit is correct, complete, and buildable before anyone spends time on copper. Go block by block (power, processor, sensors, interfaces, connectors) and check:

Power tree: every rail has a source, the regulator can supply the expected load, input and output capacitors follow the datasheet, and power-up order is handled where parts need it.
Decoupling: each IC power pin has the decoupling the datasheet calls for, with capacitor voltage ratings that leave margin.
Pin-level checks: pull-ups and pull-downs on lines that need them, unused pins handled the way the datasheet says, and no outputs driving each other.
Interfaces: voltage levels match on both sides of every bus, and any signal that leaves the board through a connector has the protection the product environment needs.
Programming and debug: a way to load and debug firmware on every programmable part, and a reset you can reach.
Parts you can actually buy: every BOM line has a manufacturer part number, a package that matches the footprint you intend to use, and a second source or an acceptable plan if it does not.
Net names and notes: clear net names and notes on anything non-obvious, so the layout reviewer is not guessing.

Then run ERC.

KiCad's documentation describes its Electrical Rules Checker as catching problems such as unconnected pins and shorted outputs, and it also notes that ERC does not detect all errors and that its quality depends on how carefully pin types were declared when the symbols were made (KiCad Schematic Editor docs).

In practice that means a clean ERC on a library with sloppy symbols proves very little. Review new or custom symbols as part of the schematic review.

PCB layout review: what to check

A PCB layout review checks that the board will fit, can be built, behaves electrically, and can be tested. For a prototype board we look at:

Mechanical fit: board outline, mounting holes, connector and switch positions, keep-outs, and component heights against the enclosure model.
Footprints: every footprint checked against its datasheet land pattern and pin 1 marking, especially new or hand-made footprints.
Placement: decoupling capacitors close to the pins they serve, switching regulators laid out the way the datasheet recommends, and sensitive parts away from noisy ones.
Power and return paths: trace widths and copper for the expected current, a continuous return path under fast signals, and thermal relief and copper for parts that get warm.
Controlled signals: if a high-speed or RF interface needs a specific impedance, the stackup and trace geometry have been agreed with the board house.
Design for test: test points on every power rail and key signals, a debug header that is reachable once the board is in its fixture or enclosure, and a way to isolate sections during bring-up. Our board bring-up checklist explains why this is the cheapest bring-up fix you will ever make.
Assembly: polarity and pin 1 marks in silkscreen, reference designators readable, fiducials if the assembler wants them, and enough space around parts for rework on a prototype.

Then run DRC against the actual capabilities of the board house you plan to use, not the tool's default rules.

KiCad, for example, lets you set rules and severities and warns that setting a rule to Ignore disables that check entirely (KiCad PCB Editor docs).

Many teams also use the board house's own DFM check on the uploaded files.

IPC-2221B, the IPC Generic Standard on Printed Board Design, is the usual reference behind many of these rules if you need to go deeper (IPC-2221B table of contents).

PCB design review checklist (copy this)

Use this as a starting point and adapt it to your board. Each line should end with a yes, a no with an action, or "not applicable" with a reason.

Before layout (schematic)

Requirements and block diagram match the schematic
Power tree checked: sources, loads, sequencing, capacitors per datasheet
Decoupling on every IC power pin, ratings with margin
Pull-ups, pull-downs, and unused pins handled per datasheet
Interface voltage levels match; external connectors protected
Programming, debug, and reset access on every programmable part
New or custom symbols reviewed; ERC clean or every waiver explained
BOM has manufacturer part numbers and buyable parts

Before routing (placement)

Outline, holes, connectors, and heights checked against enclosure CAD
Footprints checked against datasheets, pin 1 marked
Critical parts placed first (decoupling, regulators, crystals, RF)

Before release (layout + files)

Return paths, current-carrying copper, and thermal copper reviewed
Stackup and impedance agreed with the board house where needed
Test points on every rail and key signal; debug header reachable
DRC clean against the board house's rules, not defaults
Silkscreen polarity, pin 1, and reference designators readable
Fab outputs, drill files, pick and place, and BOM all from the same revision
Revision number on the board and in the file names
Review actions closed or consciously deferred, with an owner

AI schematic review: where it helps, and where it does not

AI schematic review tools can speed up the routine part of a review, especially datasheet lookups, but they do not replace ERC, DRC, or an experienced reviewer.

What these tools say they do: Flux describes its AI as checking decoupling capacitors, pull-up and pull-down resistors, power and ground connections, and component ratings against datasheets, and its documentation shows it running ERC and DRC on a project (Flux on AI design reviews, Flux design verification docs).

A 2026 comparison of AI schematic review tools published by one of the vendors in this space lists several options for KiCad, Altium, and Flux projects and makes the same point we would: the tools sit on top of ERC and a human review, and each finding should be checked against the datasheet (Cherry Blossom tool comparison).

Treat vendor claims as claims; test a tool on a board you already know before trusting it on a new one.

Where we find AI useful in a prototype review:

Pulling the relevant datasheet limits for every IC so the reviewer is not hunting through PDFs
A first pass for missing decoupling, pull-ups, or obvious rating mismatches
Summarizing what changed between two revisions so the reviewer knows where to look
Drafting the review action list from the reviewer's notes

Where a human still has to decide:

Whether the circuit meets the product's real requirements, environment, and cost target
Layout judgment: placement, return paths, thermal behavior, and fit in the enclosure
Anything the tool cannot see, such as how the board is assembled, tested, or serviced
Whether a flagged issue is real. AI tools can be confidently wrong, so every finding is a lead, not a verdict

If you are sharing design files with any outside tool, check its data terms first, the same way you would before sending files to a vendor. Our broader take on AI tools in hardware programs is in AI tools for hardware prototyping in 2026.

Who should review the board

The best reviewer is someone who did not draw it. For a prototype, a practical review group is the board designer, a second electrical engineer, the firmware engineer (who will live with the pin assignments and debug access), and the mechanical engineer for placement and fit. For larger gate decisions that cover the whole product, not just the board, use a full engineering design review.

Keep the output simple: a list of findings, each with an owner, a decision (fix now, fix next revision, accept), and a status. That list is what turns a review into fewer respins.

What to send before a PCB design review

If you want an outside team to review your board, send:

Schematic as PDF plus native files
Layout files and the stackup
BOM with manufacturer part numbers
Enclosure or mechanical CAD, or at least the board outline and key constraints
Requirements: what the board must do, power source, environment, and any certifications you expect to need
The board house and assembler you plan to use, if known
Known concerns or open questions

How LA NPDT approaches PCB design reviews

At LA NPDT, electronics, firmware, and mechanical work sit in the same team, so a PCB review is not just an electrical check. In practice:

Schematic, placement, and release reviews before a prototype order, sized to the board
The mechanical engineer checks placement against the enclosure before routing
Bring-up and test access are planned in the review, not after the boards arrive
AI tools are used for datasheet lookups and first-pass checks, and every finding is verified by an engineer
Review findings carry into design for manufacturing review, firmware testing, and the design freeze decision

If you have a board, or an idea that needs one, start with a free 20-minute call: book here. When a project needs a deeper look before any build, our Stage 1 Review/Analysis + Plan is a fixed $800 single payment. Learn more about our electronic design services and product discovery to prototype path.

Have a board you want reviewed before you order?

If you have a board, or an idea that needs one, book a free 20-minute call. When a project needs a deeper look before any build, Stage 1 Review/Analysis + Plan is a fixed $800 single payment. Phone: +1 318-200-0526.

Book a free initial consultation

Sources

Frequently asked questions

What is a PCB design review?

A PCB design review is a structured check of a board's schematic, layout, and fabrication files by someone other than the designer, done before the board is ordered, so errors are fixed in CAD instead of on built boards.

What should a PCB design review checklist include?

At minimum: power tree and decoupling, pin-level checks, interface levels, programming and debug access, footprints, mechanical fit, test points, DRC against the board house's rules, and a consistent set of fab and assembly files from one revision.

Is ERC and DRC enough for a PCB review?

No. ERC and DRC only check what the symbols and rules describe. KiCad's own documentation says ERC does not detect all errors. A human review still has to check whether the circuit meets the requirements and whether the layout will fit, behave, and be testable.

Can AI do a PCB design review?

AI schematic review tools can check things like decoupling, pull-ups, and component ratings against datasheets and can run ERC and DRC in some tools. They are a useful first pass, but findings need to be verified by an engineer, and layout and product-level judgment still need a human.

When should you review a PCB design?

Review the schematic before layout, review placement before routing, and do a release review of the finished layout and fab package right before ordering prototype boards.

How long does a PCB design review take?

It depends on board complexity and how complete the files are. A small two-layer board and a dense multilayer board with RF are very different reviews. Ask for a scoped estimate once the reviewer has seen the schematic and layout.

Tagged:AI Electronics Prototyping

Services related to this guide

PCB design review: a checklist before you order prototype boards

Boards are cheap to change in CAD and expensive to change after they ship. Here is how we review a schematic, a layout, and the fab package before a prototype order, and where AI review tools fit.

November 11, 20269 min read

Written by Konstantin Dolgan, Ph.D., NPDP

Founder & CEO, Product Development Engineer

Published November 11, 2026

What is a PCB design review?

When to run a PCB review in a prototype program

Run a short review at each point where the design is about to get harder to change. In our programs that usually means three passes:

Pass	When	Main question	Typical inputs
Schematic review	Before layout starts	Will this circuit work and can we buy the parts?	Schematic PDF, block diagram, requirements, BOM draft, key datasheets
Layout review	Placement done, then again after routing	Will this board fit, behave, and be testable?	Layout files, stackup, mechanical outline / enclosure CAD, placement notes
Release review	Right before ordering	Are the fab and assembly files complete and consistent?	Gerbers or ODB++, drill files, pick and place, BOM with manufacturer part numbers, fab and assembly notes

Schematic review: what to check

A schematic review checks that the circuit is correct, complete, and buildable before anyone spends time on copper. Go block by block (power, processor, sensors, interfaces, connectors) and check:

Power tree: every rail has a source, the regulator can supply the expected load, input and output capacitors follow the datasheet, and power-up order is handled where parts need it.
Decoupling: each IC power pin has the decoupling the datasheet calls for, with capacitor voltage ratings that leave margin.
Pin-level checks: pull-ups and pull-downs on lines that need them, unused pins handled the way the datasheet says, and no outputs driving each other.
Interfaces: voltage levels match on both sides of every bus, and any signal that leaves the board through a connector has the protection the product environment needs.
Programming and debug: a way to load and debug firmware on every programmable part, and a reset you can reach.
Parts you can actually buy: every BOM line has a manufacturer part number, a package that matches the footprint you intend to use, and a second source or an acceptable plan if it does not.
Net names and notes: clear net names and notes on anything non-obvious, so the layout reviewer is not guessing.

Then run ERC.

In practice that means a clean ERC on a library with sloppy symbols proves very little. Review new or custom symbols as part of the schematic review.

PCB layout review: what to check

A PCB layout review checks that the board will fit, can be built, behaves electrically, and can be tested. For a prototype board we look at:

Mechanical fit: board outline, mounting holes, connector and switch positions, keep-outs, and component heights against the enclosure model.
Footprints: every footprint checked against its datasheet land pattern and pin 1 marking, especially new or hand-made footprints.
Placement: decoupling capacitors close to the pins they serve, switching regulators laid out the way the datasheet recommends, and sensitive parts away from noisy ones.
Power and return paths: trace widths and copper for the expected current, a continuous return path under fast signals, and thermal relief and copper for parts that get warm.
Controlled signals: if a high-speed or RF interface needs a specific impedance, the stackup and trace geometry have been agreed with the board house.
Design for test: test points on every power rail and key signals, a debug header that is reachable once the board is in its fixture or enclosure, and a way to isolate sections during bring-up. Our board bring-up checklist explains why this is the cheapest bring-up fix you will ever make.
Assembly: polarity and pin 1 marks in silkscreen, reference designators readable, fiducials if the assembler wants them, and enough space around parts for rework on a prototype.

Then run DRC against the actual capabilities of the board house you plan to use, not the tool's default rules.

KiCad, for example, lets you set rules and severities and warns that setting a rule to Ignore disables that check entirely (KiCad PCB Editor docs).

Many teams also use the board house's own DFM check on the uploaded files.

IPC-2221B, the IPC Generic Standard on Printed Board Design, is the usual reference behind many of these rules if you need to go deeper (IPC-2221B table of contents).