Fusion PCB Specification

PCB Gerber Files


The Gerber format is an open 2D binary vector image file format. It is the standard format used by the printed circuit board (PCB) industry software to describe the printed circuit board images: copper layers, solder mask, legend, etc. All PCB orders require a set of Gerber files.

Gerber files should be inside a .rar or.zip archive with standard file extensions:

      Extension                                 Layer
  • 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


FR4 Substrate Boards

Items

DescriptionSpecs
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 size500 x 500 mm
Tolerance ± 0.2 mm
Available Board Layers1-6 layers
Available Board QtyMinimum5 pieces
Maximum8000 pieces  
Dielectric Constant
4.2 - 4.7  
Dielectric Separation thickness0.075 - 5.0






Available Board Thicknesses (mm)
1 and 2 layers0.6, 0.8, 1, 1.2, 1.6, 2, 2.5, 3 
4 layers0.8, 1, 1.2, 1.6, 2, 2.5, 3 
6 and 8 layers1, 1.2, 1.6, 2, 2.5, 3 
10 layers1.2, 1.6, 2, 2.5, 3 
12 layers1.6, 2, 2.5, 3 
14 layers2, 2.5, 3 
16 layers2.5, 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 Holes0.2 - 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

Aluminum Board Specification
No. of Circuit Layers1
Available Board Thicknesses1 mm, 1.2 mm, 1.6 mm, 2 mm
Quantity min: 5, max: 8000
Board Dimensionsmin: 10 x 10 mm
max: 500 x 500 mm
Available Board ColorsWhite (Silkscreen is black)
Black (Silkscreen is white)
Copper weight1 oz
Surface Finish HASL*, HASL lead-free,  ENIG, OSP, Hard Gold

*Contains lead, not RoHS compliant.
Minimum Trace Width/Spacing 4/4 mil
Minimum Trace Spacing 0.2 mm
Production Lead Time5 - 11 working days

Flexible PCB (FPC) Board Specification
FPC Board Specification
Layer:
1, 2
Available Board Thickness
0.1 mm, 0.15 mm
Quantity
min: 5, max: 8000
Board Dimension
max: 100 x 100 mm
Solder mask color
Yellow
Silkscreen color
White
Copper weight
0.5 oz
Surface Finish
ENIG
Minimum Trace Width
0.10 mm
Minimum Trace Spacing
0.10 mm
Minimum Drilling Hole
0.3 mm
Production Lead Time
5 - 7 working days
Temperature Range
-40℃ to 280℃

Panelization Rules:

Please click here for more details.




Modified 2019/11/25

Feedback and Knowledge Base