PCBs and Eagle CAD

Designing PCBs in Eagle CAD, a practical getting started guide.


This article provides some hints and tips on designing PCBs for successful fabrication at home by the hobbyist, taking into account the limitations of the equipment available. Guidance is provided on using the Eagle CAD software but the majority of the information is relevant to any CAD package.

The PCB production method used is, print to transparency, expose to UV light, develop, then etch.

Creative Commons License
This work is licensed under a Creative Commons Attribution 3.0 Unported License  

Other articles in the series:
Starting out with Eagle CAD
Making PCBs at Home

EagleCAD tips

When using EagleCAD for PCBs at home I use the following settings when printing the PCB for a single sided PCB.

Layers 16 (bottom), 17 (pads), 18 (vias), 20 (dimension), 45 (holes) and 116 (centerdrill) are the only layers visible.


For a SMT board routed on layer 1, layer 1 (top) would be visible and layer 16 (bottom) would be invisible.

When printing, set the scale to 1 and click 'Black' under options. If you do not set the output to black, you will get an overexposed board.

Note: I have achieved equally good results using 65 gsm tracing paper compared to 120gsm PCB transparencies. The cost of tracing paper is much less, the only difference in the process was the UV exposure time. For tracing paper I used 2 minutes, for laser transparencies I used 2 minutes 30 seconds.

To aid in drilling, I use a User Language Program (ULP) call drill-aid.ulp which is included with Eagle. This adds a new layer that 'spots' drill holes for you, it ensures that only a small section of copper is etched away and makes drilling much easier. To use it, goto File->Run then select drill-aid.ulp, click 'open' then when prompted, I normally set the drill diameter to 0.5mm.

For tracking, I use a Design Rule Check (DRC) file, homepcb.dru, if you want to use this file, save it to your EagleCAD/dru sub folder. To use this, goto Tools-> DRC.

When the menu opens, click load, then in the dru folder, part of the Eagle CAD install, you need to open the homepcb.dru file. Then click, 'Check'


This checks pad to pad, track to track spacing and many more items but is generally suitable for home use.

Tracking rules
For track widths, my narrowest track is 10 thou/0.254mm and my track to track spacing is 10 thou/0.254mm. Minimum drill size I use is 0.5mm. My results with the above design limits are consistently good. Examples of PCBs made to these design rules are shown later on.

To make the etching easier, I draw a polygon on layer 16 (or layer 1 for SMT) to cover the enitre board, then if you NAME it GND, you get a ground copper fill. Once this has been done, click the 'change' button and from the drop down menu, click 'Isolate' then select 10 thou/0.254 mm as a minimum, experiment to suit.


This sets the isolation gap between your tracking and the copper fill. Having plenty of copper, reduces the amount of time spent in the etchant and reduces the chances of over etching due to less copper to remove.

If tracking a single sided PCB, I track the wire links on layer 1, normally horizontally or vertically, so that when assembling the PCB, I print out the board at 2-3x zoom and use this to locate the wire links.

You can increase the default drill size from 0.5mm by clicking the 'Change' button, then select 'Drill' from the menu, I typically use 0.6mm hole with 0.5mm tinned copper wire.
You then need to click each via hole/pad to change the drill size.

You may find it easier to change the via shape from round to square as it gives you some more copper pad to solder too, click 'Change' then 'Shape' then Square and click each via pad.

To add text on your PCB, click the 'Text' button, enter your text but before clicking LMB to place, from the menu bar, change the Ratio to 16% and use a minimum size of 1.016 and set layer to 16 (bottom). From experimentation, this is a text size that survives home etching.


Finally, to change the measurement units or grid size, just type grid and press enter. From the menu that appears, you can set the grid spacing, 1.27mm is a good starting point, choose to display the grid as dots or lines. If you chnage the 'size' option from mm to mil (mil = thou of an inch) then all measurements in Eagle use the units from then on.

I've made 12 PCBs at home using Eagle, and a total of 41 PCB design using Eagle over the last 6/7 years so I have learnt a thing or two.

Have fun making PCBs, I hope this guide helps.


Example PCBs design and manufactured at home


This is my PC floppy adaptor PCB prototype, tracked to the design rules on this page. The copper fill was used to provide a ground plane and to reduce the amount of time spent in the etchant.


This was the prototype PCB for my ATX power adaptor. It uses a mix of surface mount and through hole components. The discretes are 1206 size and the IC is a 14 pin SOIC.

Updated 14 April 2021