Skip to main content

Flex and Rigid-Flex boards

Please keep in mind the Design-Rules on this page 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 at the IPC online store or in German, at 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.

h = height
Dynamic BendSemi-DynamicStable Bend
Bendingfrequentmax. 20x„Bend-to-Install“
Layers1-2L recommended1-4L recommended1-10L possible
Covering*PI CoverlayPI Coverlay or solder-stopPI Coverlay or solder-stop
Min. bending radius100-150 x h flex> 20x h flex10 - 20 x h flex
Copper type**RA copperED or RA copperED or RA copper

* 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

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


< 4 layers4-6 layers7-8 layers
min. distance copper - contour200µm200µm200µm
min. distance via - copper150µm200µm300µm


Flex area length4mm
Distance PTH (Via) <> Flex area1.5mm
Distance NPTH <> Flex area0.5mm

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.

Coverlay is not recommended for QFP components unless they are completely exposed!
PI CoverlaySolder-stop
Min. bridge350µm100µm
Min. clearance200µm50µm
Applicationdynamic, stablesemi-dynamic, stable
FPCB covering coverlayFPCB covering solder-stop

Pads and Vias on flexible PCBs

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 IPC-2223

ML20:1not 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 thicknessStableSemi-DynamicDynamic
min. ratio (r/h)10:120:1100:1
min. bending radius0.9mm1.8mm9mm
2 layers e.g. 190µm thicknessStableSemi-DynamicDynamic
min. ratio (r/h)10:120:1150:1
min. bending radius1.9mm3.8mm29mm
4 layers e.g. 290µm thichnessStableSemi-DynamicDynamic
min. ratio (r/h)20:150:1not recommended
min. bending radius5.8mm15mmnot 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.

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

  • drill holes or slots
  • Contour narrowing
  • Stabilization through more copper

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

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.

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.


Multi-CB can partially apply double-sided ultra-high-temperature adhesive tape from 3M to the Flex and Rigid-Flex PCBs. This allows for easy mounting during final installation. Please use an extra layer in your data for the desired position(s).

Flexible PCBs with 3M adhesive tape can be easily used in the lead-free soldering process (peak temperature 260°C, 20 sec.). The protective cover remains largely undamaged and can be easily removed. The low outgassing of the adhesive reduces the contamination of electronic components.

Technical properties

The specified adhesive tape may be replaced by a technically equivalent product depending on stock / world market situation.
Product3M 9077 tape
Adhesive0,05mm double-coated ultra high temperature acrylic adhesive
Protective cover0,09mm paper, heat-resistant
Temperature Tolerance
(short term, ≤ 20 sec.)
Adhesive: 260°C
Protective cover: 260°C
Temperature Tolerance
(long term)
Adhesive: 150°C
Protective cover: n/a
Data sheet3M 9077 Data sheet

Example - Stiffener

You can order your flexible circuit boards with a stiffener. The available thicknesses are: 0,075mm - 3,20mm.

Popular are the thicknesses0,30mmand0,20mm, e.g. forZIF connectors.

Polyimid-Stiffener: 0,025mm - 0,225mm

FR4-Stiffener: 0,075mm - 3,20mm

In the Flex PCB calculator the final thickness (incl. stiffener) is given.

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!