Skip to main content

PCB Inspection Checklist Before and After Fab

PCB inspection checklist

Every PCB design project should get some level of review, ranging from functionality design reviews with front-end engineers to a DFM review by a fabrication house. Reviews at each step in the design process are intended to identify design errors that affect functionality, manufacturability, and sourceability for long-term production. There is also a cost aspect to a design review, as it is often the case that component swaps that reduce BOM cost can be identified.

When you’re ready to perform a review with your team or a client, one way to keep everyone on track is to use a PCB inspection checklist. PCB design reviews normally happen on the front end, before sending a design into a fabrication house. A post-build design review also occurs during product development, involving further inspections of the physical board and testing the board for functionality.

In this article, we’ll look at what she be included in a PCB inspection checklist, as well as how a checklist can be part of the design and production process. Checklists sometimes get revisited post-production, when prototypes are in-hand and are being evaluated by a design team.

What Goes Into PCB Inspection

Inspection of design data must occur at multiple points in the design process. Once the initial concept is handed off to the front-end engineer for schematic capture, the design concept will have gone through several inspections during initial creation of circuits and component selection. To ensure your design is correct before entering fab and assembly, the PCB needs to be checked in three areas:

  • In the schematics
  • In the PCB layout
  • In the PCB manufacturing data

After assembly, the design should still be tested and qualified against your performance standards to ensure the device will work as intended.

Checklists can be in document format, such as in a Word document, or in a spreadsheet format with actual check boxes. Spreadsheets on a shared resource like Google Sheets are a great way to quickly copy the checklist to a new project or part number. Once the project is shared with the PCB design reviewer, a fresh checklist can also be generated and shared with the reviewer.

In the PCB Design Data

PCB design data is where design reviews and inspections begin. Creation of the design data starts with a schematic and the schematic data needs to be complete: All parts in the schematics should include:

  • Part numbers and manufacturer info with the same parameter name
  • Closed connections using only wire objects
  • Consistent GND/PWR net and symbol naming
  • Consistent I/O naming scheme
  • No missing footprints (typically applied in a library review)

In the PCB layout, layers also need to be checked to verify the design is error-free. Some items to include are:

Signal layers

  • Trace width/spacing meets fab requirement
  • Copper weight on each layer
  • Stackup symmetry
  • Trace-to-pour, pour-to-pour, pour-to-pad, etc. clearances
  • Drilled hole wall clearances
  • Vias/pads obey industry performance standard (Class 2 or Class 3/3A)

Plane/pour layers

  • Antipads around vias
  • Plane boundaries near board edge
  • Copper weight on each layer
  • Stackup symmetry

Mask layers

  • Silkscreen layers
  • Soldermask top and bottom
  • Paste mask top and bottom

Mechanical layers

  • Collisions between component bodies
  • Mechanical layers match mechanical element outlines
  • Mechanical layers for board cutouts, routed slots, plated elements
  • Expansion components (modules, etc.) have mechanical outlines
  • Components that need mechanical models or 3D bodies have them assigned

Many of these aspects can be checked using the DRC engine in your PCB design software, but only as long as the constraints were correctly defined in the system.

Silkscreen - The silkscreen layer on the PCB layout should be examined as part of general circuit board cleanup and tidiness. Most often, the silkscreen layer will need to be organized after placement and routing are finished so that all important reference designators will be confined within the board shape boundaries. You can also take some time to hide any designators that do not need to appear in the production board.

There are other pieces of information that should be added to the silkscreen layer if they are not present already: 

  • Most recent part number and revision
  • Company or producer logo
  • Lot number, serial number, etc. (usually added by the manufacturer)
  • FCC, CE, UL, ESD, and any other safety/compliance markings
  • Special legend markings indicating expansion board placement, cable placement, etc.
  • Will these be visible if the board is assembled into an enclosure or multiple-board system?

Verify these are present in the PCB layout in silkscreen layers during a review. Other problems like clearances between silkscreen elements will be caught by the DRC system in your design software.

Solder mask - The solder mask layer shows openings in the solder mask on the surfaces of the board. The very first point to check is that openings are located on component pads for SMD parts and through-hole mounted parts. Sometimes, a tenting rule can cover these parts so that the pads are no longer visible, and this will block application of solder paste, even if the paste mask layer is correct. Other things that must be applied in the solder mask layer are any openings in the solder mask required for plating copper, such as on large copper islands or RF circuits.

  • Does any tenting rule close SMD pads?
  • Are any plated areas visible through the solder mask opening?
  • Does the expansion around SMD pads create small solder mask slivers?
  • Does expansion around pads match misregistration tolerances?

Solder mask is often formed automatically by applying a solder mask expansion rule - this is exactly how tenting is applied. The table below shows some typical expansion values that should be checked. These could be applied in the footprint, but your PCB layout software might override these values, so this should be part of the inspection in the PCB.

SMD/through-hole pads


Board edge, plated features

+0.025 mm/+1 mil to +0.1 mm/+4 mil

If non-tented, +0.025 mm/+1 mil

0 mm/0 mil

Paste mask - The paste mask layer shows openings where solder paste is applied and should generally overlap with the solder mask layer. In the PCB editor, the two layers can be overlaid on each other so that the paste mask layer corresponding to solder mask openings can be identified. Paste mask openings have to be applied in the library data, but this can be overridden in the PCB layout data, so the checks should happen in the PCB layout for your project.

Paste mask layers are one area where DFA problems are hiding. In particular, paste mask layers define where solder paste will be applied, and the paste mask opening has to be sized so that the right amount of solder paste is placed into the PCB for assembly. Some problems to correct include:

  • Eliminate merged paste mask openings between components; this should flag a DRC error
  • Reduce paste mask openings where necessary on SMD components to prevent floating
  • Paste mask openings on thermal pads should be into squares

In the Manufacturing Data

Initial manufacturing data inspections are in some ways quite simple. PCB design software allows for export of manufacturing data into standard formats (Gerbers, ODB++, or IPC-2581) that can then be used in CAM tools to view the production data. Manufacturing data checks should be performed side-by-side against the PCB layout to ensure that each of the layers match. This is a simple visual check that provides simple validation that all the required layers were exported.

For assembly, the manufacturing data needs to be checked carefully against the following layers:

  • Paste mask top and bottom
  • Solder mask top and bottom
  • Drill table data

Manufacturing data (specifically layer data) also needs to be compared against a netlist for the PCB. When the netlist/wirelist export is loaded into a CAM tool with the Gerber data, this allows shorts and opens to be identified by looking at copper connections and comparing them against the netlist data. This is typically how fabricators will do an initial engineering review of the board, just to ensure that any design errors were not overlooked by the PCB designer.

PCB inspection checklist

CAM software is used to review PCB manufacturing packages before fabrication.

In Finished Prototypes

Once prototypes are finished, they need to be inspected in several ways. The most basic set of electrical and functional tests with prototypes should focus on evaluating functionality and ensuring the device just boots up. Tests come in progressively higher levels of complexity and precision, and you may need to implement some design for test practices to streamline your test procedures. Prototype testing might include:

  • Basic power-on testing
  • Flashing and specific code test cases
  • Stress tests at high power and high I/O activity

More advanced tests for production boards will include environmental testing and more advanced stress testing, such as thermal cycle testing and power surge testing. Read this other article to learn more about stress tests in PCBAs.

Continuous Improvement

Once any problems are found, they should of course be corrected in the original design files and outputs should be regenerated for the final assembly. Eventually, you may notice that your checklist is missing something, and you’re leaving yourself open to repeated errors in your design data. This might mean something is missing from your checklist. Don’t let your checklist stay static; your checklist can be a living document that evolves as your knowledge and expertise grow over time.

If there is some error or defect that is noticed repeatedly, consider adding that item to your PCB inspection checklist. As quality is continuously evaluated and new issues are identified, investigate these and try to determine the root cause. If a root cause can be determined, update your design process, quality controls, and inspection checklists to make sure these problems are not repeated.

So what should you do to ensure all identified errors are incorporated back into the PCB design data? Make another checklist! A simple checklist can be prepared based on test and inspection results following the table format below.

Issue 1

  • RefDes:
  • Cause:
  • Fix:

Issue 2

  • RefDes:
  • Cause:
  • Fix:

Issue N

  • RefDes:
  • Cause:
  • Fix:

The format above calls out everything needed to diagnose problems and fix the design. Once this type of change request checklist is prepared by the review team, it can be passed back to the original board designer for implementation in the PCB design data.

When you need to design and build the newest technology and perform thorough evaluation before production, use the complete set of CAD tools in OrCAD from Cadence to build your circuit board. Only Cadence offers a comprehensive set of circuit, IC, and PCB design tools for any application and any level of complexity. The online DRC system enables real-time verification checking across PCB layout constraints, DFM, DFA, and specialized constraints for your product.

Subscribe to our newsletter for the latest updates. If you’re looking to learn more about how Cadence has the solution for you, talk to our team of experts.