Help Center
Want to call?
+86 755 2391 9769
Please select your shipping destination & currency & Price may differ based on your Shipping destination.
| 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. |  |
| Features | Capability | Notes | Patterns |
|---|---|---|---|
| Drill Hole Size (Mechanical) | 0.20mm- 6.30mm |
Min. drill size is 0.20mm. Max. drill size is 6.30mm. |
 |
| 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. | |
| Blind/Buried Vias | Don’t support | Currently we don't support Blind/Buried Vias, only make through holes. |  |
| 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. |  |
| PTH hole Size | 0.20mm - 6.35mm | The annular ring size will be enlarged to 0.15mm in production. |  |
| 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. |  |
| Minimum annular ring | PTH | Patterns | |
|---|---|---|---|
| 1oz Copper | 0.13mm | 0.3mm |  |
| 2oz Copper | 0.2mm | 0.3mm |
| Features | Capabilities | Patterns |
|---|---|---|
| Hole to hole clearance(Different nets) | 0.54mm |  |
| Via to Via clearance(Same nets) | 0.254mm | |
| Pad to Pad clearance(Pad without hole, Different nets) | 0.127mm |  |
| Pad to Pad clearance(Pad with hole, Different nets) | 0.54mm |  |
| Via to Track | 0.254mm |  |
| PTH to Track | 0.33mm | |
| NPTH to Track | 0.254mm | |
| Pad to Track | 0.2mm |  |
| Copper weight | Min. Trace width | Min. Spacing | Patterns |
|---|---|---|---|
| H/HOZ (Inner layer) | 5mil (0.127mm) | 5mil (0.127mm) |  |
| 1oz (Outer layer) | 1/2 layers: 5mil (0.127mm) 4/6 layers: 3.5mil(0.09mm) |
1/2 layers: 5mil (0.127mm) 4/6 layers: 3.5mil(0.09mm) |
|
| 2oz (Outer layer) | 8mil (0.2mm) | 8mil (0.2mm) |
| 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 |
| 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 |
| 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. |  |
| 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 |  |
| 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 3mm. Recommended diameter of stamp hole is 0.5mm-0.8mm; Recommended distance between the two stamp holes is 0.2-0.3mm |
|
| Min. Width of Breakaway Tab | 3mm | The minimum width of breakaway tab is 3mm. For breakaway with mouse-bites, the minimum width is 5mm. |  |
| Min. Edge Rails | 3mm | If choosing panel by JLCPCB, we will add 5mm edge rails on both sides by default. |  |
JiaLiChuang (HongKong) Co., Limited, is the largest PCB prototype enterprise in Asia, with 5 Million + PCBs orders per year. JLCPCB specializes in quick PCB prototype and volume PCB production. With 14 years of PCB manufacturing experience, we’re able to provide cost effective solutions that deliver the highest reliability PCB products to customers faster.
