=== Reference ===

* [https://www.ucamco.com/en/gerber/downloads uCAMco archive] -- the home of the Gerber spec
* [http://ohm.bu.edu/~hazen/DataSheets/Gerber/ Local archive] (EDF password) of Gerber documents

=== Grids / Traces ===

* Use English measurements (mils, not mm)
 * (for metric components of course, define the footprint in mm)
* Place all components on .050 grid to start, .025 if required
* Trace width spacing minimum .006 / .006 (wider for power)
* Route on .025 grid to start, .0125 if required
* For metric / off-grid pads, route nearby then short off-angle segment to pad

''' ALWAYS WORK WITH GRID SNAP ON''' and set to a sensible value.  "Sensible"
means normally .025 for placement, no smaller than .0125 for routing.
Use smaller only for special requirements or silkscreen text placement.

=== Holes / Pads ===

* Hole sizes specified are '''finished''' which are typically .003-.004 smaller than the drill size.
* A good minimum via size is .015 pad with .005 hole.
* For thru-hole component leads, specify a hole size at least .005 largerthan the lead diameter.
* CAVEAT In vsn 4.0.7, KiCad's gerber generating code will convert slots to circular drills.

=== Silkscreen ===

* Minimum text height .040 and minimum line width .006
* Silkscreen text cannot overlap other silkscreen graphics, pads or holes
* Start with all text right-side up, rotate 90 degrees in one direction if needed

=== Useful Writeups on Footprint Design ===

* [http://www.ti.com/lit/an/sbfa015a/sbfa015a.pdf]


=== Selected PCB capabilities from mid-range houses as of June 2016 ===

|| '''Feature'''                   || '''Advanced''' || '''Sunstone''' || '''Sierra''' ||  '''JLCPCB''' || '''OshPark''' ||
|| Outer Layer Trace Width (1 oz)  ||     .005 ||     .006 ||   .003 || .0035 || .006 ||
|| Outer Layer Trace Spacing       ||     .005 ||     .006 ||   .003 || .0035 || .006 ||
|| Innner Layer Trace width (1 oz) ||     .004 ||          ||        || || ||
|| Inner Layer Trace Spacing       ||     .005 ||          ||        || || ||
|| Pad size over drill (dia)       ||     .010 ||          ||   .006 ||.006 || .010 ||
|| Pad size over finish hole       ||          ||     .018 ||        || || ||
|| Via size over drill (dia)       ||     .008 ||          ||        || || ||
|| Minimum drill (full spec)       ||     .006 ||          ||        || .008 || .010 ||
|| Minimum drill (quick proto)     ||     .010 ||     .010 ||   .008 || || ||
|| Soldermask minimum web          ||     .004 ||     .005 ||   .004 || || ||
|| Soldermask clearance (std)      ||     .002 ||          ||   .002 || || ||
||                                 ||          ||          ||        || || ||

=== Manufacturer Notes

'''Sierra''' (aka protoexpress.com) have "No Touch" service ([http://media.protoexpress.com/notouch-pcb-design-guidelines.pdf guidelines]).  Around $100 for 3 pcs 2.5x5.5 for example.

'''Advanced''' (aka 4pcb.com) has "$33 special" (min 3pcs) up to 50 in^2.  Could batch these.

'''Sunstone''' ValueProto service is around $115 plus shipping for a 2.5x3.5 board.