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
 BendingDynamic BendfrequentSemi-Dynamicmax. 20xStable Bend„Bend-to-Install“
 LayersDynamic Bend1-2L recommendedSemi-Dynamic1-4L recommendedStable Bend1-10L possible
 Covering*Dynamic BendPI CoverlaySemi-DynamicPI Coverlay or solder-stopStable BendPI Coverlay or solder-stop
 Min. bending radiusDynamic Bend100-150 x h flexSemi-Dynamic> 20x h flexStable Bend10 - 20 x h flex
 Copper type**Dynamic BendRA copperSemi-DynamicED or RA copperStable BendED 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 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

  Min. Layers
 Distance copper - contourMin.200µmLayers-
 Distance via - copperMin.150µmLayers< 4
  Min.200µmLayers4 – 6
  Min.300µmLayers7 – 8

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. bridgePI Coverlay200µmSolder-stop100µm
 Min. clearancePI Coverlay100µmSolder-stop50µm
 ColorPI CoverlayamberSolder-stopgreen
 ApplicationPI Coverlaydynamic, stableSolder-stopsemi-dynamic, stable
  PI CoverlayFPCB covering coverlaySolder-stopFPCB covering solder-stop

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 and h, the overall height of the flexible part.

Bending radius acc. to IPC-2223

  Stable Dynamic
 1LStable10:1Dynamic100:1
 2LStable10:1Dynamic150:1
 MLStable20:1Dynamicnot recommended*
Biegeradius Flexplatine IPC2223

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

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.

Flixible PCB bending area 1

Fill open regions in the bending area with blind conductors.

Flexible circuit board bending area 2

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

FPB bending area 3

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 conductors

Use curves instead of corners in the conductor trace path.

FPC curves

Ground plane

Flexible PCB 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!