Flex PCB Design Guidelines for Manufacturing

Flex PCBs offer many advantages for both the designer and the manufacturer. The FPC’s ability to be molded and bent without breakage can lead to lighter designs that take up less space, all while resisting vibrations and other disruptions from its environment. Understanding flex PCB layout techniques is essential for creating a flexible board that allows better airflow, heat dissipation, lower assembly costs, and reduced assembly errors.

Highlights:

When you design a flex board:

1. Place plated through holes (PTH) at least 0.5 mm away from the bend area.
2. Ensure stiffeners overlap the bared coverlay by 0.030” to relieve stress.
3. Opt for adhesive-less flex materials for thinner laminates to avoid issues like copper plating cracks and moisture absorption.

In this article, you’ll learn important flex PCB layout techniques.

Flex PCB layout techniques

Flex printed board design requires a slightly different approach than rigid PCBs. Below are a few guidelines to be followed when you design a flex board.

1. Calculate the bend radius based on layer count

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 allows the necessary number of bends without damaging the copper.  IPC-2223 specifies the standards for bend radius.

There are two types of flex PCBs:

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

Bend radius depends on the number of layers in your stack-up. It can be calculated using the table below.

The bend ratio is the ratio of the bend radius to the thickness of the flex circuit. A tighter bend radius increases the flex board’s failure probability. You can design a reliable flex PCB using the table below, which outlines the minimum bend ratios for various circuit types as per IPC standards.

13 tips to keep in mind when you design bend areas:

1. 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 thickness. For example, a flex circuit with a finished thickness of 0.006” will need a 0.6” minimum bend radius or 1.2” minimum bend diameter to ensure its reliability. 
3. Insert cutouts or slits with circular sections (relief holes) having radii greater than 0.75 mm to minimize the bend radius if there are no traces in the bend region. Using cutouts will reduce the amount of material that needs to be deformed, thereby increasing flexibility.
4. Avoid plated through holes and component placement within the bend area. Place plated through holes (PTH) at least 0.5 mm away from the bend area.

5. When possible, avoid 90˚ bends. Tighter bends increase circuit damage. Instead, use gradual bends that are considered safer for the circuit.
6. Place conductors smaller than 10 mils inside the neutral bend axis, where tension or compression is minimal during flexing.
7. Design conductors running through a bend such that they are perpendicular to the bend.
8. Stagger conductors in multilayer circuits to better distribute stress across the layers during bending. This reduces the risk of conductor breakage.
9. 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.

   

10. Reduce the overall thickness of the flexible dielectric material because its thickness directly influences bendability.
11. Use tear guards to reinforce the flex material along the inside bend radius. This will help prevent the flex material from tearing.

    

12. 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.

    

13. Use cross-hatch for ground and power planes to reduce copper on a plane layer, which helps increase the board’s flexibility. Typically, we recommend 0.015” wide signals with 0.025” spacing for the cross-hatched plane layers.

Check our flex and rigid-flex PCB capabilities to learn about our quick-turn FPC services.

2. Prefer using adhesive-less flex material for thinner laminates

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.

Drawbacks of using adhesive-based materials

1. The use of adhesives in rigid areas may cause cracks in the copper plating via holes because acrylic adhesives can become soft when heated.
2. These materials are prone to absorbing moisture from the environment, making them suitable for use in systems exposed to the outside environment.
3. The core thickness of adhesive-based material can be reduced after the fabrication process. This leads to dimensional error.

Why adhesive-less flex material is preferable

1. Eliminating the adhesive bond layers makes way for thinner laminates.
2. Adhesive-less copper-clad laminates have higher operating temperature ratings and higher copper peel strength.
3. These materials do not absorb moisture when exposed to the environment.

4 material selection guidelines to follow when you design a flex circuit board.

1. Stiffener: Include stiffeners for extra support for mounting components and boosting the strength of the board.
   • Use Kapton when the stiffener thickness is less than 10 mil.
2. Cladding: Use rolled annealed copper as cladding for polyimide flex cores.

   

   • Flex PCB copper comes in 0.25oz Cu ( 9 μm), 0.375 oz Cu ( 12 μm),  and 2 oz Cu (70 μm). 
   • Use minimum copper thickness of 12 μm Cu & maximum 2oz.
   • Utilize a thin copper layer for more flexibility.
3. Coverlay: Select polyimide as the primary material for coverlay.
   • It offers uniform thickness (min. 1 mil).
   • Choose min coverlay thickness based on Cu thickness.
     • 0.5 oz Cu or less- min. 1 mil,
     • 1 oz Cu min. 1.5 mil 
     •  2 oz Cu min. 3 mil
   •  Its Dk ranges from 3.2 at 10GHz.
4. Flex materials: Prefer adhesive-less materials (copper is cast directly onto the polyimide) for higher-speed applications due to their consistent results and cost-effectiveness.
   • Choose roughly 1 mil thickness of acrylic adhesives. This applies when you use adhesive-based flex material (copper is bonded to the polyimide with acrylic adhesive).
   • Alternatively, for adhesive flex core, select 1 mil (25um) adhesive and 1 mil (25um) kapton.

Sierra Circuits’ preferred flex materials

We recommend the below materials for your flex printed circuit board:

• DuPont Pyralux AP
• DuPont Pyralux LF
• DuPont Pyralux FR

Optimizing your PCB material selection is crucial for achieving the highest quality end product. Download our Material Selector Design Guide today!

PCB Material Design Guide

9 Chapters - 30 Pages - 40 Minute Read

What's Inside:

• Basic properties of the dielectric material to be considered
• Signal loss in PCB substrates
• Copper foil selection
• Key considerations for choosing PCB materials

Download Now

3. Increase the bend radius during flex trace routing for improved reliability

Flex PCB routing involves designing the pathways for electrical connections on a flexible substrate, which requires several considerations.

10 routing strategies you should know before designing a flex circuit board

2. Always opt for a larger bend radius and eliminate sharp angles. This improves the reliability of the board.

   

3. When designing multi-layer flexible PCBs, stagger traces on the front and back. 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.

   

4. Traces should also be kept perpendicular to the overall bend to eliminate the stress points that can cause trace copper breakage.

   

5. Avoid sharp corners in the flexible areas as they can lead to stress concentration and potential failure. Use rounded corners instead.

   

6. 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.

   

7. Do not design via-in-pad in flex designs, as that can damage the thin substrate during planarization. Moreover, the smaller aspect ratio of the vias does not allow non-conductive epoxy filling, as it can hamper the electrical conductivity of the vias.
8. Implement additional through-hole plating of up to 1.5 mil for rigid-flex and flex circuits to provide mechanical support from one flex layer to another. This prevents detachment of unsupported SMT pads and non-plated through holes from the substrate due to flex bending.

   

9.  Use teardrops ( an extra copper at the junction of a pad and a trace) in flex PCBs when the copper trace width transitions from wide to narrow. This helps reduce and even eliminate potential stress concentration points on the PCB.
10. Use stiffeners in areas susceptible to excessive pressures.
11. Use anchors and spurs encapsulated with coverlay to avoid trace lifting and pad peeling.

    

To know more about FPC design, read our article 7 Must-Knows for Your First Flex PCB Design.

4. Utilize teardrop-shaped vias at the transition point in the flex design

Vias are more likely to get peeled off from the flex layers. IPC 6013 standard defines various considerations related to flex vias.

8 layout techniques to reduce the risks associated with vias for flex boards

1. Use teardrop-shaped vias to connect traces or plated-through holes in flex boards. 
2. Add tabs or anchors to vias, which helps prevent 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 a 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.

5. Design larger annular rings in flex circuit board

The main purpose of an annular ring is to establish a good connection between a via and the copper trace.

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 flexible material’s dimensional stability (1000 ppm).

It is common to allow zero breaks outside the hole from the internal pad, and in some commercial parts, there may be an agreement to allow a minimum contact ring of 270 degrees.

4 considerations while placing annular rings in your flex design

1. When designing flexible printed circuit boards, allow for some misregistration between the internal pads and the drilled hole.
2. Keep the annular rings as large as possible to improve the mechanical strength of the connection. The minimum annular ring should be 8 mil for flex printed circuit boards.

Below are annular ring sizes for flex and rigid-flex PCBs

3. Consider a minimum space of 8 mil between the tracks and the drilled holes. 
4. When dealing with traces thinner than 20 mils, it is critical to consider a teardrop annular ring to enhance the board’s structural integrity against shear force and vibrations.

6. Add stiffeners in specific areas to enhance the mechanical rigidity of the flex PCB

The stiffener is an additional mechanical piece that provides mechanical support to the PCB during the assembly. Single-sided, double-sided, and multilayered flex boards can be stiffened in specific areas by adding localized rigid material.

For assembly, stiffeners can add support for mounting components. The material can increase strength, thickness, and rigidity.

4  design tips explaining when to add stiffener to your flex board

1. Consider adding stiffeners if components need to be close to the flex area. However, depending on the component size, surface mount areas do not always require a stiffener.
2. Ensure it overlaps the bared coverlay by 0.030” to relieve stress.

   

3. Apply stiffeners to the opposite side of SMT components and to the same side as the connector or through-hole components.
4. Use Kapton or FR4 materials which are commonly used for stiffeners and can be attached with thermally-cured acrylic or pressure-sensitive adhesive.

7. Place flex layers in the center of your stack-up for ease of manufacturing

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 layout techniques and capabilities are well understood.

PCB DESIGN TOOL

Stackup Designer

TRY TOOL

7 flex PCB layout techniques to consider when designing the build-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 non-bookbinding one.

   

6. Include air-gap construction method in rigid-flex. This helps eliminate flex adhesives within the rigid sections, addresses the via reliability issues, and improves the bendability of the board.
7. Use industry-standard ECAD/MCAD tools to design and customize flex/rigid-flex boards, offering an advanced toolset.

Stack-up examples

Single-layer flex stack-ups

Two-layer flex stack-ups

Multi-layer flex stack-ups

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 outside the stack-up, which increased the possibility of manufacturing problems and issues. Second, we had to ensure the board would meet the impedance requirements.

Read, how to build a flex stack-up with controlled impedance to learn about configurations used for impedance control.

We embedded the flex layers in the center of the stack-up. This protected the layers during manufacturing 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.

PCB DESIGN TOOL

Impedance Calculator

TRY TOOL

Flex PCB checklist for manufacturing

Flex drawing requirements

To successfully design a flexible PCB, it is important for you to have a basic understanding of the flex drawing requirements, which include:

1. Flex board stack-up construction and layer order
2. Dimensional drawing and tolerances
3. FPC materials to be used
4. Specifications
5. Drill symbol chart
6. Flexibility (bend radius)
7. Plating requirements
8. Testing requirements
9. Marking requirements

To know more about flex drawing requirements, read  9 drawing requirements for flex PCB design.

What to include in flex fab notes

Cover the points below 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

Include the below points 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

Work with a competent flex printed board 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. Hence, ensure that the fab house you pick produces flex boards on a regular basis. Your planned circuit density and line spacing will also affect PCB design and layout.

Always collaborate with your supplier when it comes to material selection. The material should be suitable for the environment and the application in which the FPC will operate. Flex materials themselves are pretty durable, but flex laminates may be less suitable for certain applications.

Key takeaways:

1. Determine the bend radius based on the number of times the flex PCB will bend, ensuring copper integrity.
2. Adhere to recommended bend radius-to-thickness ratios for reliable FPC design.
3. Employ design strategies such as avoiding 90˚ bends, using tear guards, and staggering conductors to enhance flexibility and reduce stress.
4. Use larger bend radii and staggered traces, and avoid sharp corners to improve reliability during flex printed board routing.
5. Incorporate teardrop-shaped vias to minimize risks associated with via peeling and cracking in flex boards.
6. Ensure annular rings are sufficiently large to strengthen connections, considering factors like misregistration and trace thickness.
7. Introduce stiffeners in specific areas to enhance mechanical rigidity, especially around mounting components.
8. Position flex layers in the center of the stack-up to simplify manufacturing, improve impedance, and enhance reliability.
9. Work closely with flex board manufacturers to select suitable materials, adhere to design rules, and ensure compatibility with intended applications.

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 layout techniques, and follow strict guidelines.

Need help designing a flex board? Post your questions and get them answered on our PCB forum, SierraConnect.