Flex PCB Capabilities
Flexible PCB Capabilities
Category | Features | Capability | Description |
|---|
Layer Count | 1-layer,2-layers,4-layers | The number of copper layers in the FPC | Rigid-flex PCBs are not yet supported. |
FPC Stack-Up | 1-Layer (25µm dielectric thickness) | FPC with copper and coverlay on the same one side only. Inner PI thickness: 25 μm |  |
2-Layer (25µm dielectric thickness) | FPC with copper on both sides. Inner PI thickness: 25 μm |  | |
1-Layer (50µm dielectric thickness) | Tear-resistant. |  | |
2-Layer (50µm dielectric thickness) | Tear-resistant. Suitable for impedance-controlled boards. |  | |
1-Layer (Transparent) | PET Thickness: 36um |  | |
2-Layer (Transparent) | PET Thickness: 36um |  | |
4-Layer | Inner/outer layer copper weight: 1/3oz, 0.5oz, and 1oz. Lamination structures: with coverlay or without coverlay. For inner layers with 1oz copper weight, coverlay is applied by default to prevent delamination and blistering during lamination. |  | |
Dimensions | Maximum Dimensions | Regular: 234 × 490 mm | Absolute limit of 250 × 600 mm allowed with edge rails – confirm with customer support before ordering. |
Minimum Dimensions | No limit, but FPCs whose dimension is smaller than 20 × 20 mm are best panelised | ||
FPC Finished Thickness | 25µm dielectric thickness FPC: 1-Layer: 0.07 / 0.11 mm 2-Layer: 0.11 / 0.12 / 0.2 mm 50µm dielectric thickness FPC： 1-Layer: 0.12 mm 2-Layer: 0.19 mm Transparent FPC: 1-Layer: 0.14 mm 2-Layer: 0.24 mm 4-Layer FPC: 0.2 / 0.25 / 0.30 / 0.35 / 0.40 / 0.45 mm | ①The thickness of the finished FPC excluding any stiffeners(If the measured area has no copper or coverlay, the finished thickness will be reduced.) ②White coverlay is 10um per side thicker than yellow/black coverlay. | |
Outer Layer Copper Weight | Single-sided: 18 μm (0.5 oz), 35 μm (1 oz) Double-sided & four-layer: 12 μm (0.33 oz), 18 μm (0.5 oz), 35 μm (1 oz) | The thickness of copper on the FPC | |
Type of Process | Dry film process with LDI (laser direct image) exposure technology | LDI provides higher accuracy than traditional LED exposure. The machines also support automatic alignment based on board size to eliminate pad offset issues. | |
Surface Finish | ENIG. Thickness: 1u" / 2u" | ENIG deposits a nickel-gold coating on exposed pads to prevent oxidation. | |
Thickness with Stiffener | Thickness with Stiffener = FPC Thickness + Stiffener Thickness | ||
FPC Thickness Tolerance | 1. Area with stiffener thickness ≤ 0.3 mm: ±0.05 mm 2. Area with stiffener thickness between 0.3-1.0 mm(including 1.0 mm): ±0.1 mm 3. Area with stiffener thickness above 1.0 mm: ±10% 4. Gold finger area: ±0.03 mm | Additional tolerance exists for stiffeners. Thicker stiffeners have larger tolerances. | |
Holes | Hole Diameter | 0.1-6.5 mm | The recommended maximum diameter for PTHs is 5 mm, if bigger may cause risks to production |
Diameter Tolerance | ±0.08 mm | Example: A 1.00 mm designed diameter is allowed to yield any physical diameter between 0.92-1.08 mm. | |
Minimum Plated Slot | 0.50 mm |  | |
Minimum Non-Plated Slot | Not limited | At least 0.2 mm copper clearance is required around non-plated slots. | |
Castellated holes are plated half-holes on the edge of an FPC. Most often used for press-soldered connectors. ① Castellated hole diameter: ≥ 0.3 mm② Castellated hole to board edge: ≥ 0.5 mm ③ Castellated hole to hole: ≥ 0.4 mm |  | ||
Min. Via hole size/diameter | ①Regular: 0.3mm/0.55mm ②Extreme for 2-layer: 0.10mm/0.3mm (extra cost required) ③Extreme for 4-layer: 0.15mm/0.35mm (extra cost required) ④Via diameter must be at least 0.2mm larger than via hole size, 0.25mm or above is better. |  | |
Traces | Annular Ring for PTH | ≥ 0.25 mm recommended, absolute limit: 0.18 mm |  |
Minimum Trace Width/Spacing (1 oz) | ① 12 μm (0.33 oz) copper: 3/3 mil (absolute limit 2/2 mil – avoid if possible) ② 18 μm (0.5 oz) copper: 3.5/3.5 mil ③ 35 μm (1 oz) copper: 4/4 mil These are regular capabilities. Contact customer support for custom capability requirements. |  | |
Trace Width Tolerance | ±20% | Example: A 0.10 mm designed trace width is allowed to yield any physical width between 0.08-0.12 mm. | |
Pad-to-Trace Clearance | ① Via ring to trace: ≥ 0.1 mm (more whenever possible) ② Exposed pad to trace：≥ 0.15 mm (more whenever possible) |  | |
NPTH to Copper Clearance | ≥ 0.20 mm | The clearance from an NPTH to traces, pads, and copper pours | |
BGA | ① BGA pad diameter: ≥ 0.25 mm ② BGA pad to trace clearance: ≥ 0.2 mm |  | |
Coverlay/ Soldermask | Coverlay Color | Yellow / Black / White / Transparent | Yellow is recommended |
Coverlay Opening | Coverlay expansion (one-sided): 0.1 mm Coverlay opening to trace clearance: ≥ 0.15 mm (more whenever possible) |  | |
Via covering | Recommended to keep coverlay over vias | ||
Coverlay Thickness | 25µm dielectric thickness FPC: ① PI: 12.5μm, Adhesive: 15μm (on 1/3oz or 0.5oz copper） ② PI: 25μm, Adhesive: 25μm (on 1oz copper） 50µm dielectric thickness FPC: PI: 25μm, Adhesive: 25μm Transparent FPC: PET: 25μm, Adhesive: 25μm Note: white coverlay is usually 13-18μm thicker per side than yellow or black coverlay. |  | |
Minimum solder bridge width | 0.5 mm minimum, i.e. solder bridge narrower than 0.5 mm will be removed. Contact customer support for any non-standard requirements. |  | |
Silkscreen | Character Height | ≥ 1mm (More in case of complex patterns or knock-out text) |  |
Character Line Width | ≥ 0.15mm (Narrower lines do not print well) | ||
Character to Pad Clearance | ≥ 0.15mm (Any silkscreen closer to a pad than this will be clipped) | ||
FPC Outline | Laser Outline | ① Copper to board edge ≥ 0.3mm ② Copper to slots ≥ 0.3mm ③ Outline tolerance: ±0.1 mm (±0.05 mm upon request) |  |
Gold Finger Pad to Board Edge Clearance | 0.2 mm. Gold fingers will be cut back if exceeding this clearance to avoid damage during laser cutting the outline. Castellated pads are exempt from this clearance. |  | |
Panels (See FPC Panel Design Guide) | ① Spacing between boards is commonly 2 mm. For boards with metal stiffeners use 3 mm instead. ② Handling edges of width 5 mm required on all four sides. Copper pour is required on these edges, with 1 mm clearance around fiducials and 0.5 mm clearance around tooling holes. ③ Fiducials: 1 mm; tooling holes: 2 mm; Fiducial centre to board edge: 3.85 mm. Add four fiducials with one offset by 5 mm or more to aid orientation. ④ Support tab width: 0.7-1.0 mm ⑤ Maximum panel size: 234 × 490 mm |  | |
Stiffeners (Detailed Introduction) | PI Stiffener | Thickness options: 0.1 mm, 0.15 mm, 0.20 mm, 0.225 mm, 0.25 mm | PI stiffeners are most often used with gold finger connectors. For example if the connector needs to be 0.3 mm thick on a 0.11 mm FPC, a 0.225 mm stiffener thickness is most suitable. |
FR4 Stiffener | Thickness options: 0.1 mm, 0.2 mm, 0.4mm, 0.6mm, 0.8mm, 1.0mm, 1.2mm, 1.6mm (bonding with adhesive under high temperature and pressure) | FR4 is usually only used on low-end products because it is prone to chipping. Avoid if possible. | |
Stainless Steel Stiffener | Thickness options: 0.1 mm, 0.2 mm, 0.3 mm | Steel stiffeners cost more but have excellent flatness and do not easily deform. This makes them good as support under SMD components. Note that since steel is slightly magnetic it should not be used with hall effect sensors or similar components. | |
3M Tape | 3M9077 (0.05 mm thick; heat-resistant) 3M468 (0.13 mm thick; not heat-resistant) tesa8854 （0.1mm thick; heat-resistant, good adhesion, recommended） | Usually used to secure FPCs after assembly | |
EM Shielding Film | 18 μm thick, black. Helps lower EMC. The recommended practice is to add soldermask openings to electrically connect ground plane with the shield films. |  | |
Bend Radius | Recommended Minimum Bend Radius | Single layer: ≥ 6× total thickness Multi-layer: ≥ 10× total thickness | Dynamic bending applications strongly recommend 1-2 layers with adhesive-less PI substrate. |
Static vs Dynamic Bending | Static Bending: Smaller radius allowed (typically 6-10× thickness) Dynamic Bending: Larger radius required (≥ 10-15× thickness recommended) | Static: Bent once or few times during assembly and remains in fixed shape. Suitable for most applications. Dynamic: Repeated bending (thousands of cycles). Use 1-2 layers + adhesive-less PI for best lifespan. Avoid placing vias/pads in bend area. | |
Design Considerations | Impedance Calculation | Core polyimide εr: 3.3 Coverlay εr: 2.9 Core polyimide thickness: 25 μm / 50 μm | Impedance measurement and control are not yet supported. Traces are only controlled for width and the customer is responsible for choosing trace widths to achieve their impedance requirements. JLCPCB provides impedance reference line widths; see details. |
EasyEDA (Highly Recommended) | EasyEDA supports a dedicated stiffener layer. The shape and thickness of stiffeners are set and embedded in the design document so they don’t need to be entered manually when ordering. See how to design FPC at EasyEDA |  | |
Other EDA Software | Put annotations on its own layer. Include the outlines of the stiffeners and indicate material and thickness. This information is not automatically parsed so stiffener options need to be set manually when ordering. Make sure that annotation text does not overlap the board area. |  | |
Other Design Constraints | Same requirements as rigid PCBs in terms of holes, traces, soldermask, and silkscreen. |
FAQs about Flexible PCB Capabilities
What substrate materials and thicknesses does JLCPCB offer for Flex PCBs?
Can stiffeners be added to selected areas only, and what materials are supported?
Does JLCPCB support 4-layer Flex PCBs? What are the limitations compared to 1-2 layers?
What is the difference between Flex PCB and Rigid-Flex PCB at JLCPCB?
How should I prepare my design files for Flex PCB ordering, especially for stiffeners and outlines?
