Flexible PCB

The bend radius is the minimum degree up to which the flex area can bend without damage. It must be properly identified early in the design. This ensures that your design allows the necessary number of bends without damaging the copper.

There are two types of FPCs:

1.  Static: These boards will flex less than 100 times in their lifetime. They will only flex during the installation process.
2. Dynamic: FPCs flex during their operation.  They are typically used in printers.

10 tips to design reliable bend areas: 

1. Clearly define the rigid and flex regions and the bend radius early in the design stage.
2. For dynamic applications, the bend radius should be 100 times the finished board thickness.
3. If there are no traces in the bend region, insert circular cutouts with radii greater than 30 mil to minimize the amount of material that needs to be deformed and increase flexibility.
4. Avoid plated through holes and component placement within the bend area. Place plated through holes (PTH) at least 20 mil  away from the bend area.
5. Avoid 90˚ bends as they increase the risk of circuit damage. Instead, have gradual bends that are considered safer for the circuit.
6. Place conductors smaller than 10 mil inside the neutral bend axis, where tension or compression is minimal during flexing.
7. Provide sufficient space between the transition point of flex and the rigid area from the bending point to minimize the stress on the flex layers.
8. Use tear guards to reinforce the flex material along the inside bend radius. This will prevent the flex material from tearing. 
9. Maintain at least 10 mil clearance between two flex regions. With inadequate clearance, adjacent flex regions may mechanically interfere with each other, leading to bending restrictions, increased stress on the material, or even tearing.
10. Use cross-hatch for ground and power planes to reduce copper on a plane layer and increase the board’s flexibility. Typically, we recommend 0.015” wide signals with 0.025” spacing for the cross-hatched plane layers.

There are two types of flex materials:

1. Adhesive-based material: The copper is bonded to the polyimide with acrylic adhesive.
2. Adhesive-less material: The copper is cast directly onto the

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.

4 material selection guidelines for your flex printed circuits: 

1. Prefer adhesive-less materials for high-speed applications due to their consistent results and cost-effectiveness. If you are choosing adhesive-based material, have acrylic adhesives of 1 mil thickness. 
2.  If you’re mounting components on flex sections, nclude PCB stiffeners for mechanical support. Use Kapton when the stiffener thickness is less than 10 mil.
3. Use rolled annealed copper as cladding for polyimide flex cores.
4. Select polyimide as the primary material for coverlay. It offers uniform thickness (min. 1 mil).

6 routing strategies you should know before designing a flex circuit board: 

1. Stagger traces when designing multi-layer flexible PCBs,. Stacked traces will not only reduce the flexibility of your circuit but will also increase stress, contributing to the thinning of copper circuits at the bend radius.
2. Keep the traces perpendicular to the bend area to eliminate the stress points that can cause trace copper breakage.
3. Avoid sharp corners in the flexible areas as they can lead to stress concentration and potential failure. Use rounded corners instead.
4. Taper down the pads towards the end at which they are connected to the traces.  This eliminates the issue where the trace entering a pad forms a weak spot, potentially causing copper fatigue over time.
5. Do not include via-in-pad in flex designs, as it can damage the thin substrate during planarization. Moreover, the smaller aspect ratio of the vias does not allow non-conductive epoxy filling, and it can hamper the electrical conductivity of the vias.
6. Implement additional through-hole plating of up to 1.5 mil to provide mechanical support from one flex layer to another.

9 ways to design reliable vias on flex boards:

1. Teardrop annular ring when dealing with traces thinner than 20 mil to enhance the board’s structural integrity against shear force and vibrations.
2. Incorporate anchors and spurs encapsulated with coverlay to avoid trace lifting and pad peeling.
3. Avoid vias in the flex section of dynamic boards, as they are at risk of cracking
4. Maintain at least 50 mil space between the vias and the stiffener’s edge. Vias are safe over a stiffener, but those placed just off its edge risk cracking.
5. Place vias at least 30 mil away from the rigid-flex/flex interface.
6. Maintain a hole-to-flex distance of 50 mil to increase the board’s reliability. This distance can be reduced to 30 mil for commercial applications. Insufficient clearance can generate undesired stress during bending and detach the via from its plating.
7. Prefer pad-only plating (button plating) for flex boards. In this process, copper is deposited only on the vias/pads, reducing the amount of copper, which increases the board’s flexibility. Further, it aids in improving etch yields in small etch patterns by allowing manufacturers to control the copper thickness. However, the extra processing steps make this expensive.
8. Keep the drill-to-copper distance of around 8 mil to achieve accuracy in layer alignment. This aids in the manufacturing process as flex materials are prone to more movement and contraction.
9. Keep the annular rings as large as possible (at least >8 mil) to improve the mechanical strength of the connection.

The stiffener is an additional mechanical piece that provides mechanical support to your PCBA. By adding localized rigid material, single-sided, double-sided, and multilayered flex boards can be stiffened in specific areas.

Request a stack-up from your manufacturer in the design phase. 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 layout techniques and capabilities are well understood.

6 design tips to build flex and rigid-flex stack-up:

1. Position the flex layers in the stack-up’s center to provide protection from exposure to outer-layer plating. This placement also simplifies manufacturing and improves impedance and control in the flex area.
2. Use an even number of layers to ensure a balanced stack-up.
3. Utilize CAD tools for virtual mock-ups during the early design phase. You can create flex board models using stiff paper or mylar.
4. Provide impedance trace details such as trace width, height, and impedance tolerance in the stack-up.
5. Use bookbinding in rigid-flex boards, allowing more flex layers to navigate tight bends without deformation. It allows the PCB to perform bends of 180˚ or more. However, a board with bookbinding costs 30% more than a standard rigid-flex one.
6. Implement the rigid-flex air-gap construction method  to eliminate the flex adhesives within the rigid sections. This method also addresses the via reliability issues and improves bendability.