Flex and Rigid-Flex boards

Please keep in mind the following Design-Rules for your Flex- or Rigid-Flex circuit boards.

For designers of flexible circuit boards we recommend the IPC-2223 Guideline / Design guidelines for flexible circuit boards, which is available from the IPC online store or in German, from the FED website.

General Design Rules for flexible PCBs

If possible, limit the number of flex layers to 1 or 2, for maximum mechanical flexibility and cost savings.

Pay attention to a symmetrical stack-up of the printed circuit board.

The flex layers continue within the rigid part as inner layers and can there be used for conductor routing.

Distinguish between dynamic (regular) and stable flexion (bend-to-install).

The minimum bending radius is usually between 1mm and 5mm. The dynamic bending stress can only be reliably ensured with single- and double-layer flexible printed circuit boards.

Dynamic Bend	Semi-Dynamic	Stable Bend
Bending	Dynamic Bend	frequent	Semi-Dynamic	max. 20x	Stable Bend	„Bend-to-Install“
Layers	Dynamic Bend	1-2L recommended	Semi-Dynamic	1-4L recommended	Stable Bend	1-10L possible
Covering*	Dynamic Bend	PI Coverlay	Semi-Dynamic	PI Coverlay or solder-stop	Stable Bend	PI Coverlay or solder-stop
Min. bending radius	Dynamic Bend	100-150 x h flex	Semi-Dynamic	> 20x h flex	Stable Bend	10 - 20 x h flex
Copper type**	Dynamic Bend	RA copper	Semi-Dynamic	ED or RA copper	Stable Bend	ED or RA copper

h = height

* Flexible solde-stop may break or peel off after 5-10x bending

** RA = Rolled copper, suitable for dynamic, flexible applications; ED = Electrolytically deposited copper , only suited for stable and semi-dynamic applications

Construction examples for flexible PCBs

Flexible circuit board construction examples

Layout guidelines

Make track-width and –spacing within the flexible part as wide as possible
At best, the transitions from wide to narrow tracks are continually rejuvenated
Rasterize ground planes (as recommended also for rigid printed circuit boards)
From 2 flex layers, shifted placement of tracks on the PCB top and bottom
Make soldering surfaces and annular rings as large as possible
Make connections of tracks and solder pads in a tear-drop, rounded style
Stiffeners (partial mechanical reinforcements, for example, in the plug-in or mounting area) can achieve final thicknesses of 0.2 mm - 1 mm

Flex

	< 4 layers	4-6 layers	7-8 layers
	min. distance copper - contour	< 4 layers	200µm	4-6 layers	200µm	7-8 layers	200µm
	min. distance via - copper	< 4 layers	150µm	4-6 layers	200µm	7-8 layers	300µm

Rigid-Flex

Scope	Minimum
Scope	Flex area length	Minimum	4mm
Scope	Distance PTH (Via) <> Flex area	Minimum	1.5mm
Scope	Distance NPTH <> Flex area	Minimum	0.5mm

Covering of flexible PCBs

Depending on the application, solder-stop or polyimide (PI) coverlay is recommended as a cover for the flexible circuit board. At best, the maximum possible values for bridge and clearance are used.

PI Coverlay	Solder-stop
Min. bridge	PI Coverlay	350µm	Solder-stop	100µm
Min. clearance	PI Coverlay	200µm	Solder-stop	50µm
Color	PI Coverlay	amber	Solder-stop	green
Application	PI Coverlay	dynamic, stable	Solder-stop	semi-dynamic, stable
	PI Coverlay		Solder-stop

Coverlay is not recommended for QFP components unless they are completely exposed!

Pads and Vias on flexible PCBs

Flexible PCB teardrops, anchore, clearance

In general, the copper adhesion in flexible circuit boards is worse than in circuit boards with standard FR4 material. It is therefore recommended to make the pads / annular rings as large as possible. To improve adhesion, anchors and teardrops can be used.

In order to increase the stability of vias on flexible circuit boards, you can implement the following measures:

Give anular rings the maximum size
Bind vias using teardrops
Use anchors to increase the film adhesion
Do not place any vias in the bending area

Calculation of the bending radius

The minimum bending radius r results from the desired application (stable/dynamic) and h, the overall height of the flexible part.

Bending radius acc. to IPC-2223

Stable	Dynamic
1L	Stable	10:1	Dynamic	100:1
2L	Stable	10:1	Dynamic	150:1
ML	Stable	20:1	Dynamic	not recommended*

*The dynamic bending can only be reliably ensured with single- and double-layer flexible printed circuit boards.

Bending radius examples

Examples of the minimum bending radius of flexible printed circuit boards with assumed thickness (see flexible circuit board layer buildup).

1 layer e.g. 90µm thickness	Stable	Semi-Dynamic	Dynamic
1 layer e.g. 90µm thickness	min. ratio (r/h)	Stable	10:1	Semi-Dynamic	20:1	Dynamic	100:1
1 layer e.g. 90µm thickness	min. bending radius	Stable	0.9mm	Semi-Dynamic	1.8mm	Dynamic	9mm

2 layers e.g. 190µm thickness	Stable	Semi-Dynamic	Dynamic
2 layers e.g. 190µm thickness	min. ratio (r/h)	Stable	10:1	Semi-Dynamic	20:1	Dynamic	150:1
2 layers e.g. 190µm thickness	min. bending radius	Stable	1.9mm	Semi-Dynamic	3.8mm	Dynamic	29mm

4 layers e.g. 290µm thichness	Stable	Semi-Dynamic	Dynamic
4 layers e.g. 290µm thichness	min. ratio (r/h)	Stable	20:1	Semi-Dynamic	50:1	Dynamic	not recommended
4 layers e.g. 290µm thichness	min. bending radius	Stable	5.8mm	Semi-Dynamic	15mm	Dynamic	not recommended

Design of bending areas

The bending area should have parallel, equal-width tracks with the same insulation resistance which are perpendicular to the bending line.

Divide wide conductor traces into narrower conductor traces within the bending area.

Fill open regions in the bending area with blind conductors.

Ensure a perpendicular path of the conductor traces to the bending axis. Avoid pads plated-through holes in the bending area.

The bending area may be optimized depending on the application.

Dynamic bending:
spontaneous and frequent bending
Optimization for dynamic bending:

drill holes or slots
copper edges at the bending location
copper stiffeners as bending aids

Stable bending:
single occurrence bending, e.g. "bend-to-install"
Optimization for stable bends:

drill holes or slots
Contour narrowing
Stabilization through more copper

For 2 or more flex layers, please ensure a shifted placement of the conductor traces on the front and back sides of the flexible portion.

2 layer flexible circuit board copper balance

Use curves instead of corners in the conductor trace path.

Ground plane

Continuous ground planes in circuit boards should always be rastered due to the copper balance. This also applies to flexible circuit boards. Especially in the flexible bending area, ground planes have to be rastered, since otherwise they break.

Your layout program normally provides a function for rastering ground planes. Find an example for rasterization in the EAGLE program here.

Processing guidelines for flexible PCBs

Because of the high moisture absorption of polyimide, flexible circuit boards must be dried (approx. 4 h at 120 ° C) prior to the placement and soldering process and processed within 8 hours!

The soldering parameters known from rigid circuit boards can usually be used.

No guarantee! Please always clarify the final parameters with your assembly partner!