Flex PCB design requires a slightly different approach than rigid PCBs. While designing a flex board, you need to consider the board outline, bending requirements, optimum material selection, stack-up, placement of copper features, and cost factors.
A well-designed flex PCB will be lightweight, robust, durable, reliable, and easy to install. Hence, it is suitable for demanding applications like aerospace, satellites, IoT, medical, and wearable devices. Flex boards offer improved endurance to vibrations and high temperatures, making them more sustainable against harsh environmental conditions.
FPCBs can provide major savings in manufacturing costs, reduce space consumption, and have lower weight. However, their design must be optimized for their materials and use cases. This article provides several useful pointers to ensure maximum reliability, manufacturability, and economy when planning out your first flex printed circuit.
Understand the bendability of your flex PCB
The flexibility feature of flex PCBs enables designers to implement them in tiny packages. It is vital to understand two things about bendability: how many times the board will be flexing, and to what extent it will flex. The number of times it can bend determines whether the PCB will be static or dynamic. A static board is considered bend-to-install and will flex less than 100 times in its lifetime. It is generally bent during the assembly process. A dynamic board‘s design needs to be more robust in nature, as flexes on a regular basis—and will need to withstand tens of thousands of bends.
The thickness of these boards depend on several factors:
- Dielectric material selection
- Copper layer count
- Base copper weight
- Adhesive thickness
Bend radius is the degree up to which the flex area of a circuit board can flex. The minimum angle the flexible region can bend must be identified very early in the design phase. This ensures that your design allows the necessary amount of bends without damaging the copper. It is calculated based on the number of layers in the PCB.
Bend ratio is the ratio of the bend radius (R) to the thickness (T) of the flex circuit. The failure probability is more if the bend radius is tighter. For a reliable flex PCB design, the minimum bend ratio for different types of circuits according to IPC is mentioned in the below table :
|Number of layers||Bend ratio for static boards||Bend ratio for dynamic boards|
Design tips when laying out the bend areas:
- Avoid 90º bends as that causes high strain. Use gradual and large curved angles that prevent circuit damage.
- Plated through-holes and placement of components should be avoided in the bend area.
- Conductors running through a bend area need to be perpendicular to the bend axis
- Stagger conductors in multi-layered circuits for greater circuit effectiveness.
- Place conductors smaller than 10 mils within the neutral bend axis where there is least tension or compression during flexing.
The thickness of the flex circuit directly influences its flexibility. Lesser the thickness, the more the pliability. Reducing copper trace thickness can increase bendability. In multilayer flex PCBs with a large layer count, it becomes difficult for the board to bend. Copper thickness can be reduced by cross-hatching the ground planes on both sides of the signal layers.
Tighter the bend radius, the higher will be the flexibility. However, the chances of damage are also more. You should understand the optimum trade-off between having a smaller radius and the extent of bending required for your flex PCB design.
If there are no traces in the bend region, the bend radius can be minimized through the insertion of cutouts or slots. Using cutouts will reduce the amount of material required to bend. Another option is removing sections of the flex where there is no circuitry, although this must be removed lengthwise and will require routing afterward.
Flex PCB Design Guide10 Chapters - 39 Pages - 45 Minute Read
- Calculating the bend radius
- Annular ring and via specifications
- Build your flex stack-up
- Controlled impedance for flex
- The fab and drawing requirements
Know your flex PCB materials
IPC 4202, 4203 and 4204 standards prescribe different materials and their specifications. You need to have knowledge about the PCB materials and their characteristics that would suit your design criteria. The properties that you need to consider are:
- Moisture absorption
- Fire retarding
- Dielectric constant (Dk)
- Glass transition temperature (Tg)
- Coefficient of thermal expansion (CTE)
Basic flex materials
Flex materials offer better material properties when compared to rigid PCBs. A flex board will have the following materials:
Dielectric insulator and coverlayer: Polyimide is the primary material used for both flex core and coverlay layers. The thickness of this dielectric flex material is uniform with an improved dielectric constant (Dk) value ranging between 2.5 to and 3.2 at 10GHz. The lack of woven glass reinforcement eliminates variations in Dk. Due to its cast manufacturing process, polyimide has an extremely uniform thickness. The typical layer thickness ranges from 0.5 to 4 mils.
Conductor: As copper foil is a good conductor, it is extensively used in making PCB circuits. Polyimide flex cores are cladded with either electro-deposited or rolled annealed copper. This copper is very thin and is suitable for both dynamic and static applications. 0.5oz (0.7mils) copper is commonly used in flex PCBs. The most common flex PCB copper weights are 0.5oz and 1oz. The maximum copper weight is 2oz. This gives the best combination of the thinnest possible construction.
Flexible copper-clad laminate (FCCL): It is a flex PCB’s core component that comprises layers of copper foil and polyimide. These boards generally use rolled annealed copper. Rolled annealed copper is created by subjecting electro-deposited copper to the rolled annealed process. It provides a tighter bend radius. The grain structure is transformed from a vertical to an elongated horizontal structure. This improves the ductility of copper, making it suitable for dynamic applications. Fully annealed or low-temperature annealed copper gives better flexing characteristics.
Bondply: These composites are made of polyimide films coated with B-staged acrylic adhesives on both sides. To encapsulate etched details in heavy copper multi-layered constructions of flex/rigid-flex boards, bondply is used in-between two conductive layers from different FCCL cores.
Adhesives: There are different types of adhesives available that are used in flex circuits – acrylic adhesives, epoxy adhesives, and pressure-sensitive adhesives (PSA) are a few of them.
PSAs are very flexible, have superior bond strength, and are easy to work with. They can adhere to the substrate or other surfaces directly. PCB adhesives can be acrylic or epoxy-based, and they’re supplied as flexible tape. They are known as thermosetting adhesive films. Applying enough pressure and heat makes the film tacky to secure the components in place. After this, they are placed in an autoclave/pressure and additional heat and pressure are applied to finalize the bond.
Acrylic adhesives stay malleable even after its cured and are a good choice for dynamic applications. Epoxy adhesives are not preferred for dynamic operations as it cures hard. In a rigid-flex PCB design, the flexible region can use acrylic adhesive and the rigid region can use epoxy adhesives.
Stiffeners: Single-sided, double-sided, and multilayer flex circuits can be stiffened in specific areas by adding localized rigid material called PCB stiffeners. This can add mechanical support for mounting components, increasing strength, thickness, and rigidity. Kapton and FR4 materials are commonly used for stiffeners. Sometimes, aluminum or stainless steel is used. These materials can be attached with thermally cured acrylic adhesive or pressure-sensitive adhesives. Stiffeners can be used for strain relief, weight balancing, and heat dissipation. They reinforce solder joints and increase abrasion resistance.
Surface finish types: There are many different types of surface finishes that provide a solderable surface and prevent copper oxidation. Choose what suits best for your flex PCB based on the application. The board surface is protected using coverlay, covercoat, photo-imaged dry film, and liquid photo-imaged polymer.
Think about the placement of preliminary components (SMT or TH) placement and determine whether those components require stiffeners. Circuitry layout makes or breaks a PCB. Important layout design and routing considerations during flex PCB design include:
- A large bend radius is preferable instead of sharp angles that shorten a board’s lifespan.
- Curved traces cause lower stress than angled ones.
- Conductors should also be routed perpendicular to the overall bend. This eliminates the stress points that can cause trace copper breakage.
- Stagger traces on the top and bottom of a flex board with two or more layers. This will avoid I-beaming due to stacked copper traces which minimizes the stress that can damage copper circuits.
- Use tear guards in the circuit to reinforce the flex material along the inside bend radius and eliminates tears.
- Transition gradually from wide to narrow traces always, tapering down the traces from the thick to the thin.
- Avoid discontinuities like vias, cut-outs, slits, and holes in the bend area. Bending a via causes stress and cracks that ultimately cause malfunctions and failures.
- Terminate cutouts/slits in flex region as per IPC standards with circular sections (relief holes) to prevent tearing at corners. The radii should be greater than 0.75mm.
- Use stiffeners in areas susceptible to excessive pressures. Use anchors and spurs encapsulated with coverlay to avoid trace lifting and pad peeling.
- Always keep special copper features, vias, and plated through holes 50-60 mils away from the transition region of a rigid-flex PCB. The region in between the flex and the rigid portion of a rigid-flex board is called a transition zone.
- Flex materials are prone to more movement and contraction during manufacturing. This makes drill to copper a crucial factor while designing your flex board. Always have the drill-to-copper distance of at least 8 mils.
- Understand if panel plating or pad-only-plating (button plating) is preferable for your flex circuit. Copper is deposited only on the vias/pads in button plating. Due to less amount of copper, button plating provides more flexibility. It allows manufacturers to control the copper thickness and improve etch yields in small etch patterns. It also facilitates controlled impedance at higher speeds as conductor traces have a consistent copper thickness, width, and spacing. It is expensive due to extra processing steps.
To learn more about flex design considerations, see avoid the common errors in flex PCB design.
Via design considerations in flex boards
While designing flex boards, it is important to understand the risks of using vias. It is possible for vias to crack or break peel in flex designs.
To mitigate this risk:
- Use teardrop (pad fillets) shaped vias to connect traces or plated through-holes in flex boards. This reduces potential stress concentration points. Fillets are appropriate when the pad diameter is larger than the width of the connecting strand.
- Keep the annular rings as large as possible. The main purpose of them is to establish a good connection between a via and the copper trace. Minimum annular ring should be 8 mils for flex PCB.
- Vias are okay over a stiffener, but vias just off the edge of a stiffener are at risk of cracking
Select a suitable flex PCB stack-up
Optimizing your flex stack-up by considering the type of application (static/dynamic), bend radius, number of layers, and overall board thickness. Consider these guidelines when designing the build-up:
- Build flex board models early in the design phase using stiff paper or mylar. Virtual mock-up models can be built using CAD tools. You can then glue the rigid sections to this using cardboard and put on the primary components. This model should fit your required form.
- Choose your materials based on this design and operating environment.
- While designing a rigid-flex board, place flexible layers in the middle to avoid slippage.
- Always try to implement an even number of layers to ensure a balanced stack-up.
- Clearly mention the thickness and impedance requirements of each layer in your build-up.
- Choose industry-standard ECAD/MCAD tools that offer a complete toolset to design, layout, and customize stack-up in flex/rigid-flex board features.
- Incorporate air-gap construction method in rigid-flex to eliminate the use of flex adhesives within the rigid sections, addressing the via reliability issues.
In high-layer count PCBs, the circuit bookbinding technique enables multilayer flex to bend in a small radius without deforming. This method is expensive but has several advantages:
- Reduces stress experienced by circuit layers, increasing shelf-life
- Compatible with all mounting processes
- Prevents the inner layers from buckling at the bend radius
- Board can perform bends of 180º
- Can be used in critical high-density applications.
Sierra Circuits’ rigid-flex manufacturing process is as follows:
- First, we process the flex layer as a two-layer flex board.
- Then we laminate the flex layers in between the rigid layers.
- The last step is milling the layers so the flex becomes visible.
Putting flex layers on the inside of the stack-up provides protection from exposure to outer-layer plating. This placement also simplifies manufacturing and improves impedance and control in the flex area.
The flex layer can be etched away from the design as part of a separate process, allowing for more protection. Below is a mini-case study.
Flex PCB stack-up design case study
This was a four-layer flex board with ZIF connectors requiring controlled impedance. The flex layers were located on the outside of the stack-up, which increased the possibility of manufacturing issues. There was also difficulty in achieving impedance requirements.
We embedded the flex layers in the center of the stack-up as shown in the figure below. This protected the layers during the manufacturing process and ensured that the less-durable flex layers were not exposed to outer-layer plating. This is how most rigid-flex stack-ups are designed. When the flex layers are on the outside, panels are harder to handle and process. This made the board more durable and easier to manufacture. It also allowed for better impedance and better control around the flex finger area.
Keeping the rigid material on the outside also allows us to manufacture what is essentially a rigid panel. The flex layers are also protected by our surface plating. However, it can cause embrittlement(/brittle fracture) and the process must be carefully controlled to prevent it.
The material used also played a large part in making this board rigid-flex instead of flex. Rigid AP (adhesive-less/high-performance) material was used, allowing for better impedance and reliability. It was a much better option than the original FR-4 material.
Controlled impedance and EMI shielding
Impedance control is required in flex stack-ups to reduce signal reflections and achieve dependable signal integrity. You must understand how to build a flex stack-up with controlled impedance while designing your board, especially for high-speed applications.
Always use EMI/RFI shielding techniques in your flex circuit to reduce noise. Controlled impedance and bend requirements are two factors to consider while selecting shielding methods. It is achieved by using copper layers, silver inks, or specialized films. In order to obtain regulated impedance values, the shield(s) must have electrical properties that meet both reference plane criteria and EMI.
Solid copper shield layers provide better shielding but less flexibility. Cross-hatched copper layers are more flexible due to reduced copper but may not provide very effective shielding. Tighter meshes provide better isolation and reduce emissions. These shields are connected to the ground through via stitching in the flex area which is a drawback. Design your circuit board by negotiating all these parameters. This shielding technique supports controlled impedance designs.
Controlled Impedance Design Guide6 Chapters - 56 Pages - 60 Minute Read
- Understanding why controlled impedance is necessary
- Stack-up design guidelines
- How to design for impedance
- Common mistakes to avoid
Follow IPC design, manufacturing, and testing standards for flex PCBs
Testing is an essential step in ensuring the integrity of your flexible printed circuit boards. To verify the quality of both your raw materials and your finished products, adhere to guidelines from the IPC, such as IPC-6013, IPC-2223, and IP-FC-234, and their respective successors. Considering these standards, the flex boards can be tested for efficiency and performance.
IPC-2221 (Generic standard on printed board design)
IPC-2221 establishes the generic requirements for PCB designing along with other forms of component mounting and interconnecting structures. This document also provides the test coupon design standards used for quality conformance testing for different board parameters.
IPC-2223 (Sectional design standard for flexible / rigid-flexible printed boards)
This document is used in tandem with the document IPC-2221. IPC-2223 establishes the design specification of the flex and rigid-flex PCBs, component mounting, and interconnecting structures. It provides guidance in many design areas such as material selection and construction, plating, conductor bend considerations, capacitance, and impedance control. It gives information on unsupported edge connectors/fingers specifications, using dual/single ZIF connectors, dielectric thickness adjustment between rigid and flexible regions.
Read IPC-2223 standards and design violations for rigid-flex boards to understand common design violations and ways to prevent them in rigid-flex PCBs.
This document provides information regarding the usage of pressure-sensitive adhesives (PSAs) for the assembly of flex PCBs. This guide provides information on adhesive types available and processes suggested for their proper use. It highlights strengths, weaknesses, limitations, and the right processes needed for creating proper assemblies/bare boards.
Circuit board testing is an application and environment-specific process. For example, aerospace and space applications require a more formidable process than consumer-oriented applications.
IPC-6013 standard provides the qualification and performance specification for flex PCBs. The current version is IPC 6013E published in 2021. This standard supersedes a number of previous IPC standards, including the original IPC-6013 from 1998. It specifies many different test methods for flex PCBs, including thermal, bend, and impedance testing. This standard also includes quality assurance provisions such as sample test coupons, guidelines for acceptance, and quality conformance tests.
This standard specifies the acceptability criteria for all classes of rigid, flex, and rigid-flex boards through visual interpretations. It provides graphical illustrations of the negotiable and non-admissible conditions that are externally or internally observed on the manufactured flex boards. The latest version is IPC 600 K released in 2020.
IPC-A-610 and IPC/ EIA J-STD001
IPC-610 is the standard for the acceptability of PCB assemblies including flex/rigid-flex boards.
IPC/EIA J-STD001 standard gives the requirements for soldered electrical and electronic assemblies.
Know the factors that affect the cost and turn-time of your flex PCB
While designing a flex board, the goal should always be to create a cost-effective product without sacrificing performance. The major cost driving factors in a flex PCB design are:
- Board size and shape
- Number of layers
- Dimensional tolerances
- Circuit construction type
- PCB grade (class)
- Thickness of the copper foil
- Size of drill holes
- Drill to copper distance
- Surface finish requirements
- Via features
- Types of stiffeners
- Plating requirements
Keep in mind these considerations during the design phase of your project. Always consult with the engineering team of your CM for the best possible design advice.
The five important factors that delay quick turn-around time of flex boards are:
- Inappropriate bend requirements
- Incomplete design data requirements
- Design related issues
- Missing ZIF connector specification
- Lack of information on flex-to-rigid transition zones
For on-time delivery of the flex boards, you need to ensure that you provide all the necessary information to your manufacturer and follow standard design specifications. Your fab drawing for flex-PCBs should not have any missing details. Information on flex materials, stack-ups, dimensions, flexibility, plating, marking and testing requirements, should all be mentioned without fail. Rigid-flex fab notes must consist of rigid notes and flex notes separately.
Choose a competent flex PCB manufacturer
When it comes to flex PCB design, you have to choose the right manufacturer who can provide the support you need. Make sure that the PCB shop you pick produces flex circuit boards on a regular basis. Ensure that they produce high-quality boards with quick turnaround times. Do not hesitate to ask about the materials they use, surface finish types, and technologies they implement.
Know your PCB supplier’s capabilities as they have their own design rules and recommendations that should be taken into account. Based on your circuit density and line spacing, they might suggest changes in layout design for an effective design solution. Consult with them to ensure that all the DFM guidelines for flex and rigid-flex are followed. This prevents errors and delays in the flex prototype. You can request them a stack-up before designing begins.
Work with your board supplier during material selection as well. The material should be suitable for your operating environment.
The assembly of flex boards can be challenging as they are not sturdy. Specialized fixtures should be created to hold them for an easy assembly process. You must ensure that the manufacturer removes all the moisture before the circuit is subjected to high temperatures. Flex circuits must be processed immediately after pre-baking or right after fabrication. Be aware of the advanced assembly and testing equipment that your manufacturer is using.
Make sure that your manufacturer has the necessary certifications and registrations. They should also be able to give you a higher quality-to-cost ratio. It is even better to visit your PCB manufacturer and see their capabilities for yourself. If you come to Sierra Circuits, we will give you a “behind-the-scenes” tour of our facilities in Sunnyvale, CA. You will learn all you need to know about our manufacturing and assembly process.
Flex and rigid-flex boards are proving their worth in innumerable applications across the globe today because of their intrinsic advantage. However, they do require careful design consideration and collaboration with your fabrication partner. Let us know in the comments section if you need any assistance in building your flex PCB. Our design and manufacturing experts will be happy to help you.