Anyone who has learned a layout package like EAGLE and sent a board off to a fab knows the trepidation felt when submitting the final gerbers. It doesn't matter if the order is for 3 PCBs or 3,000 PCBs. The time lost from an error can ruin a project's momentum, especially if it is a boneheaded error. 


Of course any PCB that is sent for fabrication should be properly reviewed. All DRC errors checked and cleared, component supplies verified with vendors, and gerbers closely inspected layer by layer. But what about footprints? Getting boards back only to find that a 44QFN component won't fit is frustrating, and even worse since cut-and-jump solutions are rarely effective with footprint errors. I don't know anyone that would jump at the chance to dead-bug a 44QFN. Reviewing each component's measurements in a library would not only be time consuming and tedious, but also not 100% effective. 


There is a better way to check all of the footprints with a layout: Paper PCB Protos. This low-tech technique only takes an hour, but can provide 100% confidence in the footprints checked. Thanks to proper scaling of the PCB, it is possible to create a PDF and print out an exact representation of the board. The designer can then place parts on the paper to quickly determine if a component's footprint will be suitable, at least for a pilot production build.

This tutorial is completed with EAGLE v6.4.0, looking at an Arduino LeonardoArduino Leonardo PCB.


Step 1: With the board file open, select the layers of interest. I like to only look at 'TOP', 'PADS', and 'DIMENSION' layers because this test is only about the copper.

01 Select Layers.jpg

Step 2: Adjust the printer settings for a 1:1 scale, and hit 'Print'. The important settings are highlighted above. Scale factor is obvious, however the area must be 'FULL' since 'WINDOW' will result in an improperly scaled printout. Also, I prefer the 'BLACK' option to be selected since a black-and-white printout will work just fine.

02 Setup Printer.jpg

Step 3: Measure the board outline to be positive that all scaling has been done correctly. 



Step 4: Place each component on the printout and verify the footprint is correct. The image above shows a 0.02” pitch 44 QFN placed on a printout from a normal desktop printer. Anything smaller would likely require the use of a laser printer. 


Step 5: Repeat steps 1-4 for the components on the bottom side of the PCB.

This technique can also be used when trying to determine the fit in a mechanical enclosure. Gluing the PCB to a piece of cardboard gives the feel of a PCB which can have holes drilled and placed into a mechanical enclosure. One could even go as far as gluing some of the taller components in to check clearances and fit. 

Thanks to the board spins saved, I suggest that this be added to any PCB review. No review is perfect, but this plugs a pretty big hole that exists in normal PCB review steps. Now submit those gerbers with confidence!