• PCB Specifications

    Features Capability Notes Patterns
    Layer count 1,2,4,6 layers The number of copper layers in the board.
    Controlled Impedance 4/6 layer, default layer stack-up Controlled Impedance PCB Layer Stackup JLCPCB Impedance Calculator
    Material FR-4 FR-4 Standard Tg 130-140/ Tg 155
    Dielectric constant 4.5(double-side PCB)

    7628 structure 4.6

    2313 structure 4.05

    2116 structure 4.25

    Max. Dimension 400x500mm The maximum dimension JLCPCB can accept
    Dimension Tolerance ±0.2mm ±0.2mm for CNC routing, and ±0.4mm for V-scoring
    Board Thickness 0.4/0.6/0.8/1.0/1.2/1.6/2.0mm The thickness of finished board.

    Thickness Tolerance

    ( Thickness≥1.0mm)

    ± 10% e.g. For the 1.6mm board thickness, the finished board thickness ranges from 1.44mm(T-1.6×10%) to 1.76mm(T+1.6×10%)

    Thickness Tolerance

    ( Thickness<1.0mm)

    ± 0.1mm e.g. For the 0.8mm board thickness, the finished board thickness ranges from 0.7mm(T-0.1) to 0.9mm(T+0.1).
    Finished Outer Layer Copper 1 oz/2 oz (35um/75um) Finished copper weight of outer layer is 1oz or 2oz.
    Finished Inner Layer Copper 0.5 oz (17um) Finished copper weight of inner layer is 0.5oz only.
  • Drill/Hole Size

    Features Capability Notes Patterns
    Drill Hole Size (Mechanical) 0.20mm- 6.30mm

    Min. drill size is 0.20mm. Max. drill size is 6.30mm.

    (Note: Blind and buried holes are not available now.)

    Drill Hole Size Tolerance +0.13/-0.08MM e.g. for the 0.6mm hole size, the finished hole size between 0.52mm to 0.73mm is acceptable.
    Min. Via hole size 0.2mm For Single&Double Layer PCB, the minimum via hole size is 0.3mm;For Multi Layer PCB, the minimum via hole size is 0.2mm
    Min. Via diameter 0.45mm For Single&Double Layer PCB, the minimum Via diameter is 0.6mm;For Multi Layer PCB, the minimum via diameter is 0.45mm.
    Pad Size 0.70mm- 6.35mm The pad hole size will be enlarged 0.15mm in production.
    Min. Non-plated holes 0.50mm The minimum NPTH dimension is 0.50mm, Please add the NPTH in the mechanical layer or keep out layer.
    Min. Plated Slots 0.65mm The minimum plated slot width is 0.65mm, which is drawn with a pad.
    Min. Non-Plated Slots 1.0mm The minimum Non-Plated Slot Width is 1.0mm, please draw the slot outline in the mechanical layer(GML or GKO)
    Min. Castellated Holes 0.60mm The minimum diameter of castellated holes is 0.60mm.
    Hole size Tolerance (Plated) +0.13mm/-0.08mm e.g. for the 1.00mm Plated hole, the finished hole size between 0.92mm to 1.13mm is acceptable.
    Hole size Tolerance (Non-Plated) ±0.2mm e.g. for the 1.00mm Non-Plated hole, the finished hole size between 0.80mm to 1.20mm is acceptable.
    Rectangle Hole/Slot Don’t support We don't make rectangle hole/slot,the rectangle hole/slot will be made as round or oval hole/slot by defalut.
  • Annular Ring

    Minimum annular ring Via Pad Patterns
    1oz Copper 0.13mm 0.2mm
    2oz Copper 0.2mm 0.25mm
  • Minimum clearance

    Features Capabilities Patterns
    Hole to hole clearance(Different nets) 0.5mm
    Via to Via clearance(Same nets) 0.2mm
    Pad to Pad clearance 0.152mm
    Via to Track 0.254mm
    Pad to Track 0.54mm
    NPTH to Track 0.25mm
  • Minimum trace width and spacing

    Copper weight Min. Trace width Min. Spacing Patterns
    H/HOZ (Inner layer) 5mil (0.127mm) 5mil (0.127mm)
    1oz (Outer layer) 5mil (0.127mm) 5mil (0.127mm)
    2oz (Outer layer) 8mil (0.2mm) 8mil (0.2mm)
  • BGA

    Layer count Min. BGA Pad Dimensions Min. Distance Between BGA Patterns
    1/2 layers 0.4 mm 0.127mm
    4/6 layers 0.25 mm 0.127mm
  • Solder Mask

    Features Capabilities Notes Patterns
    Solder mask opening/ expansion 0.05mm The solder mask should have a minimum of a 0.05 mm "growth/mask opening" around the pad to allow for any mis-registration.
    Solder bridge

    0.2mm(green)

    0.254mm(other colors)

    To have solder mask bridge, the spacing between copper pads edge must be 0.2mm (8mils) or more.
    Solder mask color green, red, yellow, blue, white, and black. We use LPI (Liquid Photo Imageable) solder mask. It is the most common type of mask used today.
    Solder mask dielectric constant 3.8
    Solder mask thickness 10-15UM
  • Legend

    Features Capabilities Notes Patterns
    Minimum Line Width 6 mil (0.153mm) Characters width less than 6mil(0.153mm) will be unidentifiable.
    Minimum text height 32 mil (0.8mm) Characters height less than 32mil(0.8mm) will be unidentifiable.
    Character width to height ratio 1:6 The preferred ratio of width to height is 1:6.
    Pad To Silkscreen 0.15mm The Minimum Distance Between Pad and Silkscreen is 0.15mm.
  • Board Outlines

    Features Capabilities Notes Patterns
    Trace to Outline 0.2mm Ships as individual board(Rounting):Trace to Outline≥0.2mm
    Trace to V-cut line 0.4mm Ship as panel with V-scoring: Trace to V-cut line≥0.4mm
  • Panelization

    Features Capabilities Notes Patterns
    Panelization without space 0mm The space between boards is 0mm.
    Panelization with space 2mm Make sure the space between boards should be ≥2mm,otherwise it will be hard to process for rounding.
    Panelized Round board ≥20mmx20mm

    The single round board size should be≥20mmx20mm.

    Panelize with stamp holes and add tooling strips on four board edges

    Panelized castellated holes board Panelize with stamp holes and add tooling strips on four board edges

    The distance between castellated hole and board corner should be larger than 2mm.

    Recommended diameter of stamp hole is 0.5mm-0.8mm;

    Recommended distance between the two stamp holes is 0.2-0.3mm

    Min. Edge Rails 3mm If choosing panel by JLCPCB, we will add 5mm edge rails on both sides by default.

We use cookies to offer you a better experience.Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site,you consent to the use of our cookies.