Coupons Download APP

Ship to

PCB Manufacturing & Assembly Capabilities

Know JLCPCB's Capabilities & Get your PCBs Built Fast

Green

Purple

Red

Yellow

Blue

White

Black

Rigid PCB

Flex PCB

PCB Assembly

SMT Stencil

Layer count	1-32 Layers	The number of copper layers in the PCB
Controlled Impedance	4/6/8/10/12/14/16/18/20/.../32 layers	User Guide to the JLCPCB Impedance Calculator JLCPCB Impedance Calculator
Impedance Tolerance	±10%
Material	FR-4	Grade A laminates from suppliers including Nan Ya, KB, Shengyi and etc.
	Aluminum-Core	1-layer Aluminum-core PCBs
	Copper-Core	1-layer copper-core PCBs with direct heatsink contacts to core (≥ 1 × 1 mm)
	RF PCB	1 oz copper, 2-layer RF PCBs with Rogers and PTFE cores
FR-4 Dielectric Constants	4.5 (2-Layer PCB)	7628 Prepreg 4.4 3313 Perpreg 4.1 2116 Perpreg 4.16
Maximum Dimensions	FR4(1-layer): 606 × 510 mm FR4(2-layer): 670 × 600 mm FR4(4-layer): 663 × 593 mm FR4(6-layer and above): 656 × 586 mm Rogers / PTFE Teflon PCB: 590 × 438 mm Aluminum PCB: 602 × 506 mm Copper PCB: 480 × 286 mm	These limits apply to PCBs with thickness ≥ 0.8 mm. The thinner FR4 PCBs are 599 × 497 mm maximum. 2-layer FR4 PCBs can reach a maximum size of 1020 × 600 mm. 4-layer FR4 PCBs can reach a maximum size of 1016 × 596 mm.
Minimum Dimensions	FR4/Rogers/PTFE: 3 × 3 mm Castellated / Plated Edges: 10 × 10 mm Aluminum/Copper PCB: 5 × 5 mm	These limits apply to PCBs with thickness ≥ 0.6 mm. Manual review required for thinner PCBs. Panelization is recommended for small-sized boards.
Dimension Tolerance	±0.1mm	±0.1mm(Precision) and ±0.2mm(Regular) for CNC routing, and ±0.4mm for V-scoring
Thickness	0.4 – 4.5 mm	Thickness for FR4 are: 0.4/0.6/0.8/1.0/1.2/1.6/2.0 mm (2.5 mm and above are for 12+ layer PCBs only)
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	2-layer: 1 oz / 2 oz / 2.5 oz / 3.5 oz / 4.5oz Multi-layer: 1 oz / 2 oz
Finished Inner Layer Copper	0.5 oz / 1 oz / 2 oz	Finished copper weight of inner layer is 0.5oz by default.
Soldermask	Green, Purple, Red, Yellow, Blue, White, and Black.	We use LPI (Liquid Photo Imageable) solder mask. This is the most common type of mask used today. Heat-cured ink soldermask is usually found on low-cost, single-sided PCBs.
Surface Finish	HASL (leaded / lead-free), ENIG, OSP (copper core boards only)	FR4 has all three finishes available, 6+ layers and RF boards only have ENIG. Aluminium core boards only have HASL. Copper core boards only have OSP.

Drill Diameter	1-layer: 0.3 – 6.3 mm 2-layer: 0.15 – 6.3 mm Multilayer: 0.15 – 6.3 mm	Holes with diameter ≥ 6.3 mm are CNC routed from a smaller drilled hole. Min. drill diameter for 2- or more-layer PCBs is 0.15 mm (more costly!) Min. drill diameter for aluminum-core PCBs is 0.65 mm Min. drill diameter for copper-core PCBs is 1.0 mm
Hole size Tolerance	Through-holes: +0.13 / -0.08 mm Press-fit holes：±0.05 mm (Finished hole size: 0.55-1.025mm. Multilayer ENIG boards only. Mention the specific holes in PCB Remark)	e.g. for the 0.6mm hole size, the finished hole size between 0.52mm to 0.73mm is acceptable. To avoid soldermask or tin stuck in the hole, recommended PTH size≥0.5mm.
Average Hole Plating Thickness	18μm
Hole Position Tolerance	±0.05 mm
Blind/Buried Vias	Not supported	Currently we don't support Blind/Buried Vias, only make through holes.
Min. Via hole size/diameter	0.15mm / 0.25mm	1-layer (NPTH only): 0.3 mm hole size / 0.5 mm via diameter 2-layer: 0.15mm hole size / 0.25mm via diameter Multilayer: 0.15 mm hole size / 0.25 mm via diameter ① Via diameter should be 0.1mm(0.15mm preferred) larger than Via hole size. ② Preferred Min. Via hole size: 0.2mm ③ 0.15mm hole size with any size via diameter, and 0.2mm or 0.25mm hole size with via diameter less than 0.45mm, will cost more. Please select corresponding via size option when placing order.
Min. Non-plated holes	0.50mm	Please draw NPTHs in the mechanical layer or keep out layer.
Min. Plated Slots Width	2-layer: 0.5mm Multi-layer: 0.35mm	The minimum plated slot width is 0.5mm, which is drawn with a pad. The length of the slot should be at least 2 times of the width.
Min. Non-Plated Slots	1.0mm	The minimum Non-Plated Slot Width is 1.0mm, please draw the slot outline in the mechanical layer(GM1 or GKO)
Slot Hole size Tolerance	Plated: +0.13 / -0.08 mm Non-plated: ±0.2mm	Plated slot is made by drill tools. Non-plated slot is made by CNC.
Via Hole-to-Hole Spacing	0.2mm
Pad Hole-to-Hole Spacing	0.45mm
Min. Castellated Holes	0.5mm	Castellated holes are metalized half-holes on PCB edges, commonly used on daughter boards to be soldered onto carrier PCBs. ① Hole diameter (Φ): ≥ 0.5 mm ② Hole to board edge (L): ≥ 1 mm ③ Hole to hole (D): ≥ 0.5 mm ④ Min. PCB size：10 × 10 mm ⑤ Min. PCB thickness: 0.6 mm
Plated Edges	10 x 10mm	Plated edges are copper-plated and ENIG treated. HASL is not supported. ① Min. PCB size: 10 × 10 mm ② Min. PCB thickness: 0.6 mm ③ At least 3 breaks (more for larger PCBs) in the edge plating are required for support tab connections
Blind Slot		① Blind slot width (W): ≥1.0mm ② Blind slot depth (D): ≥0.2mm ③ Blind slot annular width (A): ≥0.3mm (The pad width of PTH blind slots) ④ Safety distance (S): ≥0.2mm (The distance from NPTH blind slots to pad/traces/copper plane) ⑤ Blind slot remaining thickness (R): ≥0.2mm (The distance from the bottom of the blind slot to the nearest inner copper layer/surface substrate) ⑥ Supports 2-32-layer FR4 boards with a thickness of ≥0.8mm
Backdrill		Backdrill uses a secondary drilling process to control the depth of the hole, removing excess copper from the other layers of the via, thereby reducing its interference with the signal. ①Supports 4-32-layer FR4 boards with a thickness of ≥0.8mm ②Through-Hole Diaemter(D): 0.2-0.5mm(Epoxy filled after backdrilling) ③Backdrill Diameter(W): typically 0.2mm larger than through-hole diameter ④Backdrill Depth(L):layers with backdrilling, customizable ⑤Dielectric Thickness(T): ≥0.15mm(from bottom of backdrill to the adjacent inner copper layer) ⑥Safety Distance(S): ≥0.2mm(edge to pad/trace/copper safety distance)
Rectangular Holes / Slots	Not supported	Rectangular holes and slots without rounded corners are not supported.

Min. track width and spacing (1 oz)	0.10 / 0.10 mm (4 / 4 mil)	1- and 2-layer: 0.10 / 0.10 mm (4 / 4 mil) Multilayer: 0.09 / 0.09 mm (3.5 / 3.5 mil). 3 mil is acceptable in BGA fan-outs.
Min. track width and spacing (2 oz)	0.16 / 0.16 mm (6.5 / 6.5 mil)	2-layer: 0.16 / 0.16 mm (6.5 / 6.5 mil) Multilayer: 0.15 / 0.15 mm (6 / 6 mil)
Min. track width and spacing (2.5 oz)	2 layer: 0.2/0.2mm(8mil/8mil)
Min. track width and spacing (3.5 oz)	2 layer: 0.25/0.25mm(10mil/10mil)
Min. track width and spacing (4.5 oz)	2 layer: 0.3/0.3mm(12mil/12mil)
Track width tolerance	±20%	e.g. For a 0.1 mm track, the finished track width ranges from 0.08 and 0.12 mm.
PTH annular ring	≧0.20mm	2-layer: 1 oz: Recommended 0.25 mm or above; absolute minimum 0.18 mm 2 oz: 0.254 mm or above Multilayer: 1 oz: Recommended 0.20 mm or above; absolute minimum 0.15 mm 2 oz: 0.254 mm or above
NPTH pad annular ring	≧0.45mm	Recommended 0.45 mm or more. This is to allow a 0.2 mm ring of copper to be removed around the hole for the sealing film to attach. Pad sizes smaller than the recommended value can result in the annular ring being very thin or completely missing.
BGA	0.2mm	① 0.2mm-0.25mm BGA pad diameter requires ENIG ② BGA pad to trace clearance ≥ 0.1 mm (min. 0.09 mm for multilayer boards) ③ Vias can be placed within BGA pads using filled and plated-over vias
Trace coils	0.15/0.15mm	Minimum trace width/clearance: 0.15/0.15mm, when traces are covered by solder mask (1oz). Minimum trace width/clearance: 0.25/0.25mm, when traces are NOT covered by solder mask (1oz). ENIG only(high risk of short circuit with HASL)
Hatched grid width and spacing	0.25 mm
Same-net track spacing	0.25mm
Inner layer via hole to copper clearance	0.2mm
Inner layer PTH pad hole to copper clearance	0.3mm
Pad to track clearance	0.1mm	Min. 0.1 mm (stay well above if possible). Min. 0.09 mm locally for BGA pads
SMD pad to pad clearance (different nets)	0.15mm	More details of SMD pad spacing: SMD Components Minimum Spacing Minimum SMD pad: 0.25mm × 0.25mm
Via hole to Track	0.2mm
PTH to Track	0.28mm	0.35mm is recommended, minimum 0.28mm
NPTH to Track	0.2mm

READY TO GET STARTED?