This website requires JavaScript.


JLCPCB will continue production during the Lunar New Year holiday. Certain special specs will be processed after the holiday. Pls check our schedule>


Coupons
Help
Ship to

Flexible PCB Capabilities

Category
Features
Capability
Description
Layer Count
1 layer,2 layers
The number of copper layers in the FPC
Rigid-flex PCBs are not yet supported.
FPC Stack-Up
Single-Sided
FPC with copper and coverlay on the same one side only. Inner PI thickness: 25 μm
flex PCB Capability - /ssr/img/Single-Sided.1d6c391.png
Double-Sided
FPC with copper on both sides. Inner PI thickness: 25 μm
flex PCB Capability - /ssr/img/Double-Sided.ef6dd8d.png
Dimensions
Maximum Dimensions
Regular: 234 × 490 mm
Absolute limit of 250 × 500 mm allowed with mandatory handling edges – 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

Single-sided: 0.07 / 0.11 mm

Double-sided: 0.11 / 0.12 / 0.2 mm

The thickness of the finished FPC excluding any stiffeners(If the measured area has no copper or coverlay, the finished thickness will be reduced.)
Outer Layer Copper Weight

Single-sided: 18 μm (0.5 oz), 35 μm (1 oz)

Double-sided: 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
±0.05 mm
Additional tolerance exists for stiffeners. Thicker stiffeners have larger tolerances.
Holes
Hole Diameter
0.15-6.5 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
flex PCB Capability - /ssr/img/Minimum_Plated_Slot.f08c651.png
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 mm

② Castellated hole to board edge: ≥ 0.5 mm

③ Castellated hole to hole: ≥ 0.4 mm

flex PCB Capability - /ssr/img/Hole_to_board_edge.892a998.png
Min. Via hole size/diameter

0.15 mm (Via hole size)/ 0.35 mm (Via diameter)

① Annular ring: 0.1 mm minimum, 0.125 mm recommended

② Recommended via size: 0.3 mm inner, 0.55 mm outer

flex PCB Capability - /ssr/img/Via.58735d3.png
Traces
Annular Ring for PTH
≥ 0.25 mm recommended, absolute limit: 0.18 mm
flex PCB Capability - /ssr/img/pth.e7cac0f.png
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.

flex PCB Capability - /ssr/img/width_spacing.3019160.png
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)

flex PCB Capability - /ssr/img/pad_to.d2fb3e4.png
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

flex PCB Capability - /ssr/img/bag.6b51ae7.png

Coverlay/

Soldermask

Coverlay Color
Yellow / Black / White
Yellow is recommended
Coverlay Opening

Coverlay expansion (one-sided): 0.1 mm

Coverlay opening to trace clearance: ≥ 0.15 mm

(more whenever possible)

flex PCB Capability - /ssr/img/Coverlay_Opening.8b6f859.png
Via covering
Recommended to keep coverlay over vias
Coverlay Thickness

① PI: 12.5 μm, glue: 15 μm (on 12/18 μm copper)

② PI: 25 μm, glue: 25 μm (on 35 μm copper)

flex PCB Capability - /ssr/img/Coverlay_Thickness.a50f70a.png
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.
flex PCB Capability - /ssr/img/Minimum_solder_bridge_width.17d69f0.png
Silkscreen
Character Height
≥ 1mm (More in case of complex patterns or knock-out text)
flex PCB Capability - /ssr/img/Silkscreen.f2a4bae.png
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)

flex PCB Capability - /ssr/img/Laser_Outline.a825c14.png
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.
flex PCB Capability - /ssr/img/Gold_Finger.178d6c0.png
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

flex PCB Capability - /ssr/img/Panels.6096973.png
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
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)

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 over edge guard rails to electrically connect them to the shield films.
flex PCB Capability - /ssr/img/EM_Shielding_Film.3dc6f8e.png
Design Considerations
Impedance Calculation

Core polyimide εr: 3.3

Coverlay εr: 2.9

Core polyimide thickness: 25 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.
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
flex PCB Capability - /ssr/img/EDA.e3b3cdc.png
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.
flex PCB Capability - /ssr/img/Other_EDA_Software.41e13e3.png
Other Design Constraints
Same requirements as rigid PCBs in terms of holes, traces, soldermask, and silkscreen.
READY TO GET STARTED?