In this webinar, we discuss flex PCB design guidelines for manufacturing. Flex PCBs offer many advantages for both the physical designer and the manufacturer. The ability of the flex PCB to be molded and bent without breakage can lead to smaller designs that are lighter and take up less space all while resisting vibrations and other disruptions from its environment. Furthermore, they allow better airflow, heat dissipation, lower assembly costs, and a reduction in assembly errors.
What is a flex PCB?
Flex PCBs are flexible circuits with very thin substrates and high levels of bendability, tensile strength, and physical flexibility. They can also be molded into complex three-dimensional shapes for use across a diverse range of applications, such as heads-up displays for aerospace piloting and wearable technology.
What are flex PCBs made of?
Flex PCBs materials are made of acrylic base. These materials offer a lower dielectric constant when compared to rigid PCB materials. The thickness of the flex PCB materials varies between 0.5 and 5mils.
What are flex circuits used for?
Medical application: Flex PCBs are widely used in medical devices as they are compact and can have 360-degree bendability.
Automotive application: The inherent resistance of flex PCBs to vibration makes them ideal for the harsh environment inside a motor vehicle.
Space application: Most aerospace applications make use of flex boards to reduce the overall weight of the system.
Advantages of flex PCBs
Flex PCBs offer a variety of advantages for designers and manufacturers. In this section, let us have a look at a few advantages of flex PCBs.
Ease of use
- Design constraints are minimal. PCBs can be designed to fit any device shape.
- Range of motion allows PCBs to suit nearly any application.
- Reduces potential failure points found in standard PCB assemblies.
- Reduces weight through the elimination of additional wires, cables, and connectors.
- Flex enables the miniaturization of devices.
Possible cost reduction
Using flex boards can result in direct and indirect cost savings.
Direct cost savings
A single rigid-flex PCB with 6 rigid sections can replace the entire assembly of 6 rigid PCBs within the product. It eliminates wire harnesses and connector pairs. This inventory reduction leads to direct cost savings.
Indirect cost savings
Since there is no requirement for wiring harnesses the assembly cost is cut down. Excluding wiring harnesses eliminates wiring errors hence the product is more reliable. This also reduces the overall installation cost.
Static or dynamic application
Flex PCBs can be either static or dynamic. The amount of times a PCB can bend determines whether the board is static or dynamic. We will learn more about static and dynamic flex PCBs in the next section.
Flex PCB design guidelines and rules
Flex PCB design requires a slightly different approach than rigid PCBs. Below are a few guidelines to be followed when you design a flex PCB.
Understanding how your board will bend
Knowing the number of times your flex PCB will bend is crucial for your design. If a PCB is bent more times than the design allows for, then the copper will begin to stretch and crack.
Static board: A static board is considered bend-to-install, and will flex less than 100 times in its lifetime. These boards will only flex during the installation process.
Dynamic board: A dynamic board is a flex PCB that is regularly flexed and twisted. These boards generally flex during their operation. The printer is one of the most common applications where dynamic flex PCBs are used.
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
The bend radius is the minimum amount of bendiness for the flex area. It must be properly identified early in the design. This ensures your design can allow for the necessary number of bends without damaging the copper. IPC-2223 specifies the standards for bend radius.
To help determine how thick you can make your circuit, you should calculate the bend radius. This can be done based on how many layers your design has. The bend radius can be calculated using the below table.
|Number of layers||Bend radius (mils/mm)|
|1 (single-sided)||Flex thickness x 6|
|2 (double-sided)||Flex thickness x 12|
|Multi-layer||Flex thickness x 24|
Designing bend areas: Best practices
Consider the following points when you design bend areas:
- Define the rigid and flex regions and the bend radius
- Add cut-outs and slots in the bend area to increase the flexibility
- When possible, avoid 90˚ bends. Tighter bends increase circuit damage.
- Gradual bends are safer for the circuit.
- The bend radius is measured from the inside surface of the bend.
- Place conductors smaller than 10 mils inside the neutral bend axis, as they tolerate compression better than stretching.
- Avoid plated through-holes within the bend area.
- Conductors running through a bend need to be perpendicular to the bend.
- Stagger conductors in multilayer circuits to increase the effectiveness of the circuit.
Know your flex materials
There are two major types of flex PCB materials:
Adhesive-based material: The copper is bonded to the polyimide with acrylic adhesive.
Adhesive-less material: The copper is cast directly onto the polyimide.
The use of adhesives in rigid areas can create cracks in via plating. This is because acrylic adhesives become soft when heated. Consequently, when designing for adhesive-based materials, it’s important to incorporate anchors and teardrops in your design.
Advantages of using adhesive-less materials
- Eliminating the adhesive bond layers make way for thinner laminates.
- Adhesive-less copper-clad laminates have higher operating temperature ratings and higher copper peel strength.
- These materials do not absorb moisture when exposed to the environment.
Disadvantages of using adhesive-based materials
Here are a few disadvantages of using adhesive-based materials:
- The use of adhesives in rigid areas may cause cracks in the copper plating via holes because acrylic adhesives can become soft when heated.
- These materials are prone to absorb moisture from the environment. Hence it is suitable to use this type of material in a system that is exposed to the outside environment.
- The core thickness of adhesive-based material can reduce after the fabrication process. This leads to dimensional error.
Sierra Circuits’ preferred materials
We recommend the below materials for your flex PCB:
- DuPont Pyralux AP
- DuPont Pyralux LF
- DuPont Pyralux FR
PCB Material Design Guide9 Chapters - 30 Pages - 40 Minute Read
- Basic properties of the dielectric material to be considered
- Signal loss in PCB substrates
- Copper foil selection
- Key considerations for choosing PCB materials
Watch your flex trace routing
Always opt for a larger bend radius.
There is a requirement of having sharp angles, it is always recommended to have a larger radius. This improves the reliability of the board.
Use curved traces instead of traces with corners. Curved traces cause lower stress than angled ones.
When designing multi-layer flexible PCBs, stagger traces on the front and back. Stacked traces will not only reduce the flexibility of your circuit, it will increase stress contributing to the thinning of copper circuits at the bend radius.
Traces should also be kept perpendicular to the overall bend.
To know more about flex PCB design, read our article 5 Must-Knows for Your First Flex PCB Design.
Optimize your stack-up
Request a stack-up from your manufacturer before designing begins. It is crucial that you know what stack-up you are designing. Rigid-flex is the simplest configuration that will allow you to reduce the number of connectors, which will also increase wiring density and reliability.
Having a face-to-face meeting with the supplier is the best way to ensure that you’re on the same page in terms of where the overall PCB process is headed. This meeting can also help ensure that flex PCB design guidelines and capabilities are well-understood.
Place the flex layers in the center of the stack-up
For rigid-flex PCBs, we process the flex layer as a two-layer board and laminate it between the rigid layers. Placing 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.
Flex design case study
Stack-up sent by a customer:
This was a four-layer flex board with ZIF connectors requiring controlled impedance. The high-speed ZIF connectors connected finger areas from the edge to the top of the board. This stack-up had a few issues. First, the board’s flex layers were located on the outside of the stack-up, which increased the possibility of manufacturing problems and issues. Second, we had to make sure the board would meet the impedance requirements.
Also read, How to Build a Flex Stack-Up with Controlled Impedance
We embedded the flex layers in the center of the stack-up. 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 harder to 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.
The flex layers are also protected by our surface plating. The material used also played a large part in making this board rigid-flex instead of flex. Rigid AP material was used, allowing for better impedance and reliability. It was a much better option than the original FR-4 material.
What are flex PCB stiffeners?
The stiffener is an additional mechanical piece that provides mechanical support to the PCB during the assembly. Single-sided, double-sided, and multilayered flex PCBs can be stiffened in specific areas by adding localized rigid material. The material can increase strength, thickness, and rigidity.
For assembly, stiffeners can add support for mounting components. You should consider adding stiffeners if components need to be close to a flex area. But depending on the component size, surface mount areas do not always require a stiffener. You should apply stiffeners to the opposite side of SMT components and to the same side as the connector or through-hole components.
Kapton and FR4 materials are commonly used for stiffeners and can be attached with thermally-cured acrylic or pressure-sensitive adhesive.
Stiffeners should overlap the bared coverlay by 0.030” to relieve stress.
Single-layer flex stack-ups
Two-layer flex stack-ups
Multi-layer flex stack-ups
Annular rings in flex design
Annular rings in rigid-flex and flex multilayers are often compromised, especially in places where tight hole-to-pad ratios are demanded. This is mainly due to the dimensional stability (1000ppm) of the flexible material. It is common to allow zero breaks out of the hole from the internal pad, and on some commercial parts, there is sometimes agreement to allow a 270-degree minimum contact ring.
When designing flexible printed circuit boards, allow for some misregistration between the internal pads and the drilled hole. Consider minimum space between the tracks and the drilled holes.
Placing vias in a flex design
Vias are at a greater risk of getting peeled off from the flex layers. Consider the following points to reduce the risks associated with vias.
- Make annular rings as large as possible.
- Vias should be tear-dropped. Teardrops can reduce potential stress concentration points on the PCB.
- Adding tabs or anchors to vias, as shown below, will also help prevent peeling.
- Vias are not reliable in areas that will bend.
- In a dynamic application, flexed vias can crack very quickly.
- Vias are okay over a stiffener, but vias just off the edge of a stiffener are at risk of cracking.
- Vias should be placed at least 30 mil away from the rigid-flex/flex interface.
Work with your manufacturer
Understand that flex and rigid-flex design rules are different. Flex designs require button plating and annular rings need to be larger. Each manufacturer has its own set of design rules and recommendations. PCB design and layout will also be affected by your planned circuit density and line spacing.
Another thing you should always work with your supplier on is material selection. The material should be suitable for the environment and the application in which the flex PCB will operate. Flex materials themselves are pretty durable, but flex laminates may be less suitable for certain applications.
Flex checklist for manufacturing
Flex drawing requirements
To successfully design a flexible PCB, it is important for the designers to have a basic understanding of the flex drawing requirements.
The flex drawing requirements are:
- Flex PCB stack-up construction and layer order
- Dimensional drawing and tolerances
- Flex PCB materials to be used
- Drill symbol chart
- Flexibility (bend radius)
- Plating requirements
- Testing requirements
- Marking requirements
To know more about flex drawing requirements, read our article: 9 drawing requirements for flex PCB design.
What to include in flex fab notes
Below points should be covered in your flex fab notes
- Indicate that the PCB shall be fabricated to IPC-6013
- The flexible copper-clad material shall be IPC-4204/11
- The covercoat material shall be per IPC 4203/1
- The maximum board thickness shall not exceed (your requirement here) and applies after all lamination and plating processes.
What to include in your rigid-flex fab notes
Below points should be covered in your rigid-flex fab notes:
- The rigid-flex fab notes must consist of rigid notes and flex notes
- The thickness of acrylic adhesive through the rigid portion of the panel shall not exceed 10% of the overall construction
- Vacuum press in autoclave or vacuum lamination
- Misregistration between any two layers shall not exceed ±0.005’’
- Warpage shall not exceed 0.75%
- Impedance trace details such as trace width and impedance
In order to benefit from all that flex PCBs have to offer, you must have a clear vision of the printed circuit board’s functionality, familiarize yourself with the design rules, and follow strict guidelines.