PCB Design Review Checklist: What to Check Before Ordering Your First Boards
Your first custom PCB order is exciting and slightly nerve-racking. The boards take time to arrive, and a mistake you could have caught on screen becomes a pile of boards you can't use.
This checklist covers what to review before you click "order." It draws mainly on two neutral sources: the KiCad 9.0 PCB Editor manual and a PCB verification checklist used in Purdue University's ECE477 senior design course. The examples use KiCad terms, but the ideas carry over to other tools.
It deliberately gives no trace widths, clearances or drill sizes. Those come from your board maker, and they differ from one maker to the next.
Before you start: is it time for a custom board?
A custom PCB makes sense once breadboard and module experiments have answered your riskiest questions. If you're still testing whether the core idea works, a dev board is usually cheaper and faster. Our guide to where a custom board fits among prototype stages can help you decide.
1. Load your board maker's rules first
The KiCad manual recommends establishing your design rules at the start of a layout, not the end. The Constraints section of Board Setup "should be set to the values recommended by your board manufacturer." Those values are absolute minimums: no net class or custom rule can go below them.
Checklist:
- Find your board maker's published capabilities and copy them into your constraints.
- Write down where the numbers came from (page link and date), so you can recheck them if you switch makers.
2. Understand what DRC can and can't tell you
The design rule checker compares your board against the rules you configured. A clean DRC means the board follows your rules. It doesn't mean those rules match what your board maker can build. That's why step 1 matters.
KiCad's DRC dialog has two options worth turning on:
- Refill all zones before performing DRC. The manual warns that leaving it off "may result in incorrect DRC results if zones have not been refilled manually."
- Test for parity between PCB and schematic. This flags differences between the schematic and the board, such as footprints that are missing or duplicated.
3. Check the board outline and copper zones
- Closed outline. KiCad needs the shapes on the Edge.Cuts layer to form closed outlines whose endpoints coincide exactly, with no overlaps or self-intersections. Otherwise DRC reports "Board has malformed outline." Closed shapes inside the outer edge are treated as cutouts.
- Zones filled before output. Copper zone filling is manual by default in KiCad. Zones must be refilled after any change inside them, and only filled copper appears in manufacturing data. Zones also only fill inside the board outline.
4. Leave solder mask and paste expansion at zero (unless told otherwise)
The KiCad manual says most commercial fabricators expect solder mask and paste clearance values to be zero and make their own adjustments in their CAM process. Its advice is to keep the default of zero unless you're making the board yourself or your maker specifically tells you to change it.
5. Print it at 1:1 and check the physical fit
The Purdue checklist asks you to confirm all parts fit on a 1:1 scale printout of the PCB. Place real components on the paper where you can. Then check:
- Space and height. Is there room around every part's pins and pads? Has the height (z) of every part been accounted for?
- Mounting holes. Is there clearance for the bolt heads? Are the holes free of traces and other electrical items?
- Connectors. Are they on the board edges where needed, overhanging where appropriate, and facing the right way?
6. Review parts, placement and routing
From the Purdue checklist, condensed:
- Parts complete. Main components, power regulation and battery management, the support parts each datasheet or application note calls for, plus a programming header, reset circuit, power connectors, mounting holes and indicator or debug LEDs.
- Placement. Oscillator close to the microcontroller. Decoupling capacitors close to or under the ICs they serve. Parts grouped by subsystem.
- Routing. Everything routed. Oscillator traces clear of noisy signals. Trace widths suitable for the current they carry, power traces included. No acute angles.
- Ground. Analog ground separated from the main ground net where the microcontroller datasheet calls for it.
- Radio modules. If the board carries a pre-certified Wi-Fi or Bluetooth module, follow its integration instructions for antenna placement and layout, because its FCC grant assumes them. See checking a module's grant and integration instructions, and what FCC modular approval leaves to the host maker.
7. Know what a "checkerboard" layout means on a PCB
"Checkerboard" shows up in PCB guidance in a few specific places. In the sources we checked, it never means arranging the whole board in a grid. If a datasheet or design guide asks for one, check which of these it means:
- Power and ground pins and vias under large FPGAs. AMD's UltraScale PCB design guide explains that the inductance of a power connection drops when opposing currents run close together, such as a VCC via next to its GND via. That is why the core VCC pins of those FPGAs "are placed in a checkerboard arrangement in the pinout." The guide notes that the FPGA pinout determines the PCB via arrangement. What the board designer controls is mainly the stackup: keeping the power planes close to the top of the board keeps the current-carrying part of those vias short.
- Large exposed thermal pads. Analog Devices' ADC layout note AN-1142 recommends splitting a big exposed pad (EPAD) "into equal segments like a checkerboard," using a silkscreen crosshatch or solder mask, so there is a solder connection in each segment, rather than possibly only one small connection, or one in a corner. Each segment gets ground vias, and the note says to fill those vias "with solder paste or epoxy before assembly" so the pad's solder doesn't flow into them.
Checklist:
- Use the IC maker's own land pattern and via guidance when it gives one. It takes priority over general advice.
- If you split a thermal pad or put vias in it, ask your board maker and assembler how they handle via filling or plugging, and note their answer with your other rules.
- Don't add a checkerboard pattern the datasheet doesn't call for.
8. Make the silkscreen useful
The Purdue list asks for labels on every component and connector signal, placed near parts but not on pads. Mark pin 1 of every IC and the polarity of diodes and other polarized parts. Add a board name and a revision number or date, because you'll be glad of them when two versions sit on your bench.
9. Generate outputs carefully, then inspect them
- Layers. When plotting Gerbers, the KiCad manual says to check that every layer used on your board is enabled. Disabled layers are not plotted.
- Drill files. Generate them along with the Gerbers, in the format your maker recommends.
- View the output. The Purdue checklist's final step is to inspect the Gerbers in a Gerber viewer (it names gerbv) to catch defects introduced during CAM processing. KiCad also ships its own Gerber Viewer.
- Assembly files. If you're ordering assembled boards, KiCad notes your maker may require component placement (pick-and-place) files. A bill of materials (BOM) can also be exported. If your maker accepts IPC-2581 or ODB++, either can replace the separate Gerber, drill and placement files.
Keep the exact files you sent with the order. They are also the files a factory will ask for later on.
10. Record the review
For each revision, note the rules source, the checklist results, anything you couldn't verify and what you changed. Keep a dated log of each board revision so the next spin starts from facts, not memory.
Synthetic example, made up for illustration: a first sensor board passes DRC, but a 1:1 printout shows a USB connector set back from the board edge. The fix is a quick move in the layout. Found after the order, it would have meant a new revision.
FAQ
What should a PCB design review checklist include?
Board maker rules loaded as constraints, a DRC with zones refilled and schematic parity checked, a closed board outline, 1:1 footprint and mechanical checks, placement and routing review, clear silkscreen, and an inspection of the final Gerber and drill files.
If DRC passes, is my board ready to manufacture?
Not necessarily. DRC only checks the rules you configured. If those don't match your board maker's capabilities, or zones weren't refilled, DRC can pass on a board that has problems.
Should I change solder mask or paste expansion?
Usually not. The KiCad manual says most commercial makers expect zero and adjust it themselves, unless they tell you otherwise.
What files do I need to order assembled boards?
Typically Gerbers and drill files, plus component placement files and a BOM. Some makers accept IPC-2581 or ODB++ instead of separate files. Always check your maker's requirements.
How do I check Gerber files before ordering?
Open them in a Gerber viewer such as gerbv or KiCad's Gerber Viewer and look at each layer for missing copper, a broken outline, and stray or missing silkscreen.
Start your first project
ThingWeave is a pilot workspace where you and your AI agent keep requirements, sources, review notes and decisions for a hardware project in one place, so every board revision has a record of what was checked and why it changed.
Sources
- KiCad 9.0 PCB Editor Reference Manual (Board Setup constraints, design rule checker, board outline, zones, solder mask/paste, fabrication outputs): https://docs.kicad.org/9.0/en/pcbnew/pcbnew.html
- Purdue University ECE477, Systematic PCB Verification Approach (PDF): https://engineering.purdue.edu/ece477/Course/Process/PCBVerificationChecklist.pdf
- AMD, UltraScale Architecture PCB Design User Guide (UG583), FPGA Mounting Inductance: https://docs.amd.com/r/en-US/ug583-ultrascale-pcb-design/FPGA-Mounting-Inductance
- Analog Devices, AN-1142: Techniques for High Speed ADC PCB Layout: https://www.analog.com/en/resources/app-notes/an-1142.html
Sources 1–2 accessed October 19, 2026; sources 3–4 accessed October 21, 2026.