• pcbname.GTL               Top Copper 
• pcbname.GTS               Top Soldermask
• pcbname.GTO               Top Silkscreen
• pcbname.GBL                Bottom copper
• pcbname.GBS                Bottom Soldermask:
• pcbname.GBO                Bottom Silkscreen:
• pcbname.TXT                 Drills
• pcbname.GML/GKO       Board Outline
• pcbname.GL2                 Inner Layer 2 (for ≥ 4 layer)
• pcbname.GL3                 Inner Layer 3 (for ≥ 4 layer)

Notes:
1. Gerber files should be in RS-274X format (RS-274D is not recommended due to issues reading the files).
2. Drill file (PCBname.TXT) should be in Excellon format.
3. Gerber file and Drill file (PCB name.TXT) should be included in the same folder.
4. The board outline is required, ideally in an isolated mechanical layer.

Standard Seeed Fusion PCB Service Specification

Items	Description	Specs
		Units: mm or mil as specified
Board Dimension	Min size	10 x 10 mm Tip: If your board width is smaller than this size, you can make a bigger panel and use slots to separate the board.
	Max size	500 x 500 mm
	Tolerance	± 0.2 mm
Available Board Layers	1-6 layers
Available Board Qty	Minimum	5 pieces
	Maximum	8000 pieces
Dielectric Constant		4.2 - 4.7
Dielectric Separation thickness		0.075 - 5.0
Available Board Thicknesses (mm)	1 and 2 layers	0.6, 0.8, 1, 1.2, 1.6, 2, 2.5, 3
	4 layers	0.8, 1, 1.2, 1.6, 2, 2.5, 3
	6 and 8 layers	1, 1.2, 1.6, 2, 2.5, 3
	10 layers	1.2, 1.6, 2, 2.5, 3
	12 layers	1.6, 2, 2.5, 3
	14 layers	2, 2.5, 3
	16 layers	2.5, 3
	Tolerance	± 10%
Available Board Copper Weight		1 oz. 2 oz. 3 oz.
Surface Finish Options		HASL*, HASL lead-free, ENIG, OSP, Hard Gold *Contains lead, not RoHS compliant.
Minimum trace spacing / width		[Spacing/Width] mil For 1 oz: 4/4 mil, 5/5 mil, 6/6 mil For 2 oz: 10/10 mil For 3 oz: 15/15 mil *Minimum trace/width spacing for RF coil designs is 6/6 mil, but please select the 4/4 mil option.
Minimum trace width in inner layers (for 4 layers board)		≥ 6 mil
Minimum distance between vias (plated holes)		≥ 12 mil To prevent ion migration
Minimum distance between plated holes and trace		≥ 12 mil To prevent ion migration
Annular Rings		≥ 0.1 mm (4 mil) for vias ≥ 0.152 mm (6 mil) for PTH
Outer Layer Copper Thickness		0.035 - 0.07 mm (1 oz - 2 oz)
Inner Layer Copper Thickness		0.017 mm (0.5 oz)
Drill Hole Diameter (NPTH)		0.2 - 6.3 mm  (larger sizes will be milled)
	Size Tolerance	± 0.05 mm
	Position Deviation	± 0.05 mm
Plated Hole Diameter	Via Holes	0.2 - 0.5 mm (0.3mm and smaller vias can guarantee full solder mask tenting)
	Plated Through Holes (PTH)	0.2 - 5.8 mm (larger sizes not guaranteed)
	Castellated Holes (Plated Half-Holes)	≥ 0.50 mm
	Size Tolerance	± 0.075 mm
CNC Milling/Routing	Non-Plated Milling Slot Width	≥ 0.8 mm
	Plated Milling Slot Width	≥ 0.65 mm
	Milling/Routing Tolerance	± 0.15 mm
Width of Solder Mask Dam		Normal: ≥ 0.32 mm for Green ≥ 0.35 mm for Other colors Please select 0.1mm option: ≥ 0.10 mm for Green ≥ 0.13 mm for other colors
BGA size		≥ 0.45 mm pitch BGAs (select 6/6 mil trace width/spacing) ≥ 0.35 mm pitch BGAs (select 5/5 mil trace width/spacing) ≥ 0.25 mm pitch BGAs (select 4/4 mil trace width/spacing)
Circuit to edge		≥ 0.3 mm
Minimum distance between inner trace and plated holes		≥ 0.2 mm / 7.87 mil
Minimum silkscreen height/trace width		Height ≥ 0.5842 mm / 23 mil Trace width ≥ 0.1016 mm / 4 mil *Smaller widths are possible but we cannot guarantee print quality.
Ideal silkscreen aspect ratio		1:5
Silkscreen color		Silkscreen color is WHITE   when solder mask is Green, Red, Yellow, Blue, Black Silkscreen color is BLACK when solder mask is white
Pad to Silkscreen Clearance		≥ 0.1524 mm / 6 mil
V-Cut / V-Score / V-Groove (V-cut lines must go across the entire length of the boards, i.e. no jump cuts.)	Board Length (both sides)	55 to 380 mm
	Sub-Board Dimensions	≥ 8 x 8 mm
	V-Cut Line Width	0.4 mm (0.8mm to trace clearance required i.e. 0.4mm from the centre of the v-cut line)
PCB production time (build time)		3 - 14 working days *Depends on specific order parameters as calculated on the order form

Please click here for more details.