PCB Design Checklist

Prevent costly iterations by finding mistakes before ordering

Use this checklist to systematically review your PCB design before sending it to production. Your progress is automatically saved in your browser.

Overall progress: 0 / 0

1. Schematics Check

0/9

Not-connected pins: Check all NC pins. Are you sure they shouldn't be connected? MCU pin verification: Verify microcontroller pins with datasheet (pinmuxing/pinconfig). Watch out for open-drain pins, current ratings, slew rate. Connector grounding: For each connector/mounting hole: are all shield/GND pins connected to GND? Page settings: Issue date, revision, title, and layout template are filled in correctly. ERC: Run the Electrical Rules Check. Fix each issue where possible, but be careful before adding 'no connect' or power flags. Bidirectional components: For bidirectional symbols (e.g., TVS diodes, non-ceramic capacitors): is the selected component actually bidirectional? Protection: Are all connectors sufficiently protected against EMC/ESD and miswiring/short circuit risk? Bus addresses: If an I2C bus is used with multiple devices, check for conflicting addresses. Prevent backpowering:Check that signals connecting to potentially powered-down circuitry do not create parasitic leakage paths. Inrush current: Are switches/relays/inputs sufficiently protected against inrush current? (e.g., switching large capacitance may need slew-rate limiting)

2. Layout Check: Placement

0/5

3D view: Review the 3D view for overlapping parts or parts that are so close that they would be hard to place. Mating connectors: For each connector/mounting hole: is the mating connector/screw/cable going to fit? Sometimes the cable-side connector is wider than the PCB footprint! Enclosure fit: Is the board outline compatible with the final product/enclosure? Export the PCB to CAD software and try to fit it. Assembly sequence: Is it possible to assemble the board into your product? Visualize the assembly order: watch out for notches in the PCB outline and connectors extending past the board outline. Sensor orientation: Check for each sensor if the orientation with relation to the physical world is correct (e.g., direction of an encoder strip).

3. Layout Check: Routing

0/6

High-contrast review: Review each layer in high-contrast mode: can traces be made nicer/tidier? Power nets: Highlight power nets: could they be routed shorter? Are traces wide enough for the rated current? Grounding vias: Placed near signals switching layers? Sufficient stitching vias if multiple ground planes are used? DRC: Run the Design Rule Check and fix all issues if possible. Carefully review unavoidable errors (e.g., courtyard) and mark them as excluded. EMC filters: Layout is compact, near the EM source, and routed away from potential victim signals. High-speed signals: Verify length is matched correctly (if applicable).

4. Layout Check: Ground Plane

0/4

Re-pour planes: Re-pour all planes in the design (KiCad: b, Altium: t,g,a). Coverage: Verify that the ground plane covers the complete board. Correct net: Check if ground planes are connected to the correct net. Minimize cutouts: Review ground plane(s): cutouts/holes/slots should be minimized. Verify there are no slots caused by groups of vias.

5. Layout Check: Silkscreen

0/4

Readability: Silkscreen text should be clearly readable, not overlapping. Connector labels: Verify presence of clear labels for connectors (add pinout info where possible). Branding: Verify presence of company/project logo + correct PCB name/version. Latest version: Latest customer/project logo + version number on silkscreen?

6. Layout Check: DFM

0/6

Connector changes: If connectors have been replaced/removed since a previous revision: check impact on customer/assembly partner. Fine-pitch paste: In-house assembly: Reduce paste volume for <0.65mm pitch chips (-5-10%). Panel: In-house assembly: For board qty > 5, a panel with alignment holes must be present. Fiducials: Verify that at least 3 fiducials are present. Suggested size: 1mm with 2mm mask opening (for small PCBs they can be left off / placed on panel edge). Fabrication layer:Verify the fabrication layer is neat and readable: each component should have a designator. Remove extra text such as values to keep it neat. Impedance documentation: If impedance controlled tracks are present, document them on a separate layer (e.g., Cmts.User). Special requirements: Document other special requirements (conformal coating, flex PCB stiffeners) on separate gerber layers.

7. Gerber Check

0/3

Required layers: Are all required layers exported as gerber file? Are there any non-required layers (remove them to avoid confusion)? Solder mask: Are all pad openings as expected? You want solder mask between all pads if possible (KiCad: setup - pads to mask clearance: tweak clearance + min width). Paste layers: Are all required stencil openings present? Reversely, are there any openings that shouldn't be there? Usually this is a matter of footprint settings.

8. Manufacturing Documentation

0/1

README.txt: A README.txt must be present with the full board specs.

Include at least (specify 'any' if no specific requirements apply):

PCB color, size, surface finish
Layer count
Copper thickness for each layer
Thickness + dielectric of each layer
Impedance control ('none' or reference a gerber layer with detailed descriptions)
For flex PCB: top/bottom stiffener thickness + gerber layer with outlines
Special gerber layers if applicable (e.g., conformal coating)

9. BOM Check

0/4

Duplicate lines: Minimize duplicate BOM lines (e.g., same resistor in 0402 and 0603). Ratings: Is the column 'rating' properly filled in? (for high-voltage or precise passives) Accessories: Are all connectors and accessories (enclosure, add-on modules etc.) on the BOM? Pick & place: Are all components in the pick & place file (if applicable)?

Need help with your PCB design?

We can review your design or take care of the entire process from concept to production-ready PCB.

Design Review PCB Design Service