A Brief introduction to Flex and Rigid-Flex PCBs
May, 2025
This White Paper written by: Sriya Dupakuntla, Hardware Engineer II
This White Paper reviewed and edited by: Kamesh Durvasula, Engineering Manager
Introduction
Printed Circuit Boards or PCBs for short, are one of the most common building blocks for present-day electronics. A PCB provides both a “base” for components to rest on and the necessary interconnects between them. PCB design requires electrical, mechanical and manufacturing inputs and review to result in a feasible product. This paper presents an overview of aspects that need to be considered in Flex and Rigid-Flex design. It assumes some background in rigid-PCB design.
Construction of a PCB:
PCBs are multilayered stacks of copper foil and various insulating materials. The choice of copper foil, insulating material, and the number of layers determine the flexibility of a PCB.
Commonly available PCB constructions
(a) Rigid PCB (b) A Flex PCB (c) A Rigid-Flex PCB
1. Rigid PCBs:
Most rigid PCBs are built around FR4, a fiberglass weave and epoxy resin composite. This material, when hardened and cured forms the core. When hardened but not yet cured, it forms prepreg, the “glue” to stack multiple copper layers prior to curing.
Sample stack up of a 4 layer Rigid PCB
The PCB built with the stack up above consists of copper layers 2 and 3 laminated on the FR4 substrate. The outer layers are formed by laminating prepreg and copper sheets on the core. The solder mask, a paint like polymer coating is applied to this stack up. This protects the copper on the outer surfaces, and it also helps with the soldering process in exposing only specific sections of the pads and reducing the risk of solder bridges.
A section of the PCB with the solder mask scraped off reveals the copper and FR4 material beneath.
2. Flex and Rigid-Flex PCBs:
The flexible part of a flex or rigid flex PCB consists of a thin copper layer on a flexible substrate. This building block can be single or double sided and the copper can either be rolled-annealed or electro deposited on to the substrate. This substrate is typically polyimide and various thicknesses of this material are used for coverlay and stiffener layers.
Sample stack up of a 2 layer Flex PCB
A Flex PCB would consist solely of a combination of the flexible core/copper layers with a coverlay and stiffener.
The Flex PCB built with the above stack up will have two layers of copper on either side of a polyimide substrate. The Coverlay serves a similar purpose to that of solder mask for rigid PCBs. In this stack up it is a polyimide sheet glued on to the top and bottom layers with a suitable adhesive.
Sample stack up of a Rigid Flex PCB
A Rigid –flex PCB will consist of a Rigid part built of something like FR4 interleaved with the polyimide/copper layers extending into a section that is only flex. As shown in the above stack up, the flexible part of the Rigid-Flex runs through the whole PCB.
Materials
1. Substrate:
Polyimide is one of the most common materials used in FPC PCBs. There are other constructions and substrate materials available such as resin coated copper and liquid crystal polymer with suitable bonding sheet that can be used for suitable applications. For the purpose of this paper, we assume polyimide substrates.
Polyimide sheets can come in adhesive and non-adhesive variants. They can also have copper foil on a single side or both sides.
Electro deposited copper is an economical solution but rolled annealed copper might be a better choice for assemblies subject to repeated flexing. Polyimide substrates (with adhesives) absorb more water than rigid materials, this requires Flex and rigid-flex PCBs to be baked before assembly. Additional adhesive can cause cracks in vias and reduce flexibility.
Copper and film thicknesses for a Polyimide based circuit material by Panasonic:
Felios Polyimide(R-F775/R-F770)
https://www.dupont.com/electronics-industrial/laminates.html#headingacc1
2. Coverlay:
Coverlay is a thin insulating film used to cover the exposed copper on the top and bottom layers of an FPC cable. Typically, thin sheets of polyimide are used for this purpose. “Kapton” is a well-known range of polyimide sheets manufactured by Dupont.
3. Adhesive:
Adhesives used for FPCs can be epoxy, acrylic, polyurethane etc. There are options for pressure-sensitive, thermosetting and UV curable materials available as well. The thermal characteristics of the adhesive need to be considered if the flex PCB will be subject to a soldering process.
*blind-buried vias?
4. Stiffener:
Stiffeners are typically added to sections of the FPC that will have components soldered to it. These stiffeners can be polyimide, FR4, stainless steel or aluminum.
Some pcb fabricators provide material selection tools that the designer can use to make a suitable choice.
Layout considerations for Flex regions:
1. Bend Radius:
The bend radius is often an input from the mechanical and industrial design of the product. This is an important factor when creating the stack up for a flex PCB. The choice of layers and thickness determines to what extent this requirement can be met. Thinner the stack up and fewer the layers achieve tighter bends.
FPCs can have two bend applications:
- Static: The bend occurs only during installation and the board is likely to stay in this position.
- Dynamic: The FPCs bend and straighten several times during their life.
2. Material impact on bend radius:
Think substrate and copper layers increase flexibility.
Rolled Annealed copper’s grain structure makes it more suited for repeated flexing.
Non-adhesive copper polyimide stack ups are thinner and increase flexibility.
Thinner cover lay improves flexibility.
3. Layer Count impact on bend radius:
Image courtesy sierra circuit
Bend regions of a two-layer FPC with FR4 stiffener on either end
4. Layout recommendations for bend regions:
- Copper traces tolerate elongation better than compression and must be placed on the outer surface of the bend where possible.
- Avoid plated through holes in the bend region.
- Traces should be routed perpendicular to the bend axis
- Bend region should be located at a minimum distance from the rigid to flex transition.
- For multi layered PCBs, stagger the traces on either side of the flex to reduce mechanical stress.
5. Signal Integrity:
A copper pour is provided in rigid PCBs to provide a ground path for traces in adjacent layers. The typical choice for FPCs/Rigid-FPCs is to provide a copper-hatch although for certain static bend applications a solid copper pour might be feasible.
Copper hatch at 90 degrees Copper hatch at 45 degrees
Traces with a copper hatch on the layer below.
In cases where impedance matching is desired, orienting the copper hatch at 45degrees to the traces will provide better matching. As with rigid boars, the thickness of the layers will be a factor.
6. Shielding:
Shielding can be accomplished by adding additional copper layers in the FPC stack up or using specialized shielding films or inks. Silver ink offers higher flexibility, is economical in higher volumes but expensive for prototyping.
7. Routing:
Trace bends should be rounded where possible.
Preferred Acceptable
8. Vias:
Vias should be tear dropped to reduce stress and preferably tabbed to reduce peeling.
Avoid vias in the flex zone if possible. If required, place away from bend zone.
9. PCB shape
Provide rounded corners with a 20mil radius where possible
10. Land patterns:
For components that will be soldered onto the flex PCB, the land pattern should be modified to extend under the cover lay if possible. A polyimide cover lay will be machined for footprint openings. A minimum web thickness of 20mil will be required.
11. Layout considerations for the Rigid to flex transition zone:
Vias on the rigid section should be a minimum of 50 mils away from the transition zone.
Manufacturing Files
Care must be taken to ensure the manufacturing files such as gerbers and fabrication/assembly notes
Account for a flex/rigid-flex design.
1. Gerbers:
If possible, provide separate Gerber outlines for rigid and flex sections, stiffener, cover lay layers. Some manufacturers accept DXF outlines if gerbers are unavailable.
2. Fabrication Drawing:
- Fabrication drawing must provide clear stack up and material choice. Avoid trade names and specify materials per IPC standard.
- Hole sizes with dimensions and plating requirements.
- Board outline with dimensions.
- Silkscreen/coverlay /surface finish requirements.
- Provide a clear indication of the rigid section and flex section.
- Provide notes for strain relief where required. Discuss with manufacturer a need for adding epoxy in the transition zone to flex.
- Add clear indication of stiffener location and material choice.
- Indicate cover lay outline and specify material where possible.
- Fabrication notes should point to the right IPC standard. IPC-6013 has specifications for flex and rigid-flex PCBs.
- The specifications for plated through holes and vias are different for flex /rigid-flex PCBs compared to rigid PCBs and must be discussed with the manufacturer
- Add mouse bites for rigid sections and solid tables for pure flex areas. Rope in assembly house if different than fab.
Stack up options for flex and Rigid-Flex PCBs:
- For Rigid-flex, prefer flex regions in center of stack.
- Air gapped construction to reduce deformation in multi layered flex.
- Bookbinding is an option for PCBs meant to flex in a particular orientation.
It is crucial for flex and even more so for Rigid-flex to run the stack up and material selection by the manufacturer as early into the design process as possible.
Author Biography
This White Paper written by:
Sriya Dupakuntla
Hardware Engineer II
This White Paper reviewed and edited by:
Kamesh Durvasula
Engineering Manager
About Vantage MedTech
Vantage MedTech provides comprehensive design and manufacturing services, supporting the advancement of medical technologies from concept through to product realization.
Partnering with the world’s most innovative MedTech start-ups and largest medical device companies, we offer feasibility support, product development and prototyping, strategic planning for new product implementation, clinical and commercial manufacturing, and after-market services to support every phase of the product life cycle.
Our clients can leverage our proprietary Advantage Platforms®, accelerating product development timelines. Our manufacturing approach is structured to serve the changing needs of our clients, supporting small-quantity clinical or First-in-Human builds and can scale to accommodate full launch quantities.
Copyright
This White Paper contains a variety of copyright material. Some of this is the intellectual property of the author, some is owned by Vantage MedTech. Some material is owned by others which is shown through attribution and referencing. Some material is in the public domain. Except for material, which is unambiguously and unarguably in the public domain, only material owned by Vantage MedTech and Vantage MedTech, and so indicated, may be copied, provided that textual and graphical content are not altered and the source is acknowledged. Vantage MedTech reserves the right to revoke that permission at any time. Permission is not given for any commercial use or sale of the material.
Disclaimer
Whilst Vantage MedTech has attempted to ensure the information in this White Paper is as accurate as possible, the information is for personal and educational use only and is provided in good faith without any express or implied warranty. There is no guarantee given to the accuracy or currency of information contained in this White Paper. Vantage MedTech does not accept responsibility for any loss or damage occasioned by use of the information contained in this White Paper.
