Grids / Traces

• Use English measurements (mils, not 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.

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

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

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