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 China and a high-tech manufacturer specializing in quick PCB prototype and small-batch PCB production. With Over 10 years of PCB manufacturing experience, we’re able to provide cost effective solutions that deliver the highest reliability PCB products to customers faster.
