Flex PCB Design Guide: Flexible & Rigid-Flex Circuit Best Practices

After spending over a decade working with flex circuits across aerospace, medical devices, and consumer electronics, I’ve learned that flex PCB design isn’t just a variation of rigid board design—it’s a completely different discipline. The materials behave differently, the failure modes are unique, and the design rules that keep your boards reliable require careful attention to mechanical stress, bend performance, and layer construction.

This guide covers everything you need to know about flex circuit design and rigid flex PCB design, from calculating bend radius to avoiding the mistakes that cause field failures. Whether you’re designing your first flexible circuit or looking to improve your existing designs, you’ll find practical, tested guidance here.

Understanding Flex PCB Types and Applications

Before diving into design rules, let’s establish what we’re actually building. Flexible printed circuits come in several configurations, each suited to different applications and design requirements.

Single-Sided Flex Circuits

Single-sided flex is the simplest and most cost-effective option. One conductive copper layer sits on a flexible polyimide substrate, covered by a protective coverlay. These work well for simple interconnects, LED strips, and applications where routing complexity is minimal.

Double-Sided Flex Circuits

Double-sided flex adds a second conductive layer, connected through plated through-holes (PTHs) or vias. This configuration handles moderately complex routing while maintaining good flexibility. Most bend-to-install applications use double-sided construction.

Multilayer Flex Circuits

When routing density demands it, multilayer flex stacks multiple conductor layers with flexible dielectric between them. The trade-off is reduced flexibility—more layers mean a thicker cross-section and larger minimum bend radius. Dynamic applications rarely exceed four layers for this reason.

Rigid-Flex PCB Construction

Rigid flex PCB design combines rigid FR4 sections with flexible polyimide ribbons in a single integrated assembly. The rigid areas carry components and connectors while the flex sections allow three-dimensional folding and dynamic movement. This eliminates connectors between separate boards, reducing failure points and improving reliability in applications like laptops, cameras, and medical implants.

Flex Circuit Type	Typical Layer Count	Best Applications	Relative Cost
Single-Sided	1	Simple interconnects, LED lighting	Low
Double-Sided	2	Bend-to-install, moderate routing	Medium
Multilayer Flex	3-6	High-density static flex	Medium-High
Rigid-Flex	4-12+	3D assemblies, component mounting	High
HDI Rigid-Flex	6-18+	Advanced miniaturization	Very High

Critical Materials for Flex Circuit Design

Material selection directly impacts flexibility, thermal performance, and long-term reliability. Getting this wrong causes premature failures that are expensive to diagnose and fix.

Base Substrate Materials

Polyimide (PI) dominates flex circuit manufacturing for good reason. It handles temperatures up to 260°C, has excellent chemical resistance, and maintains flexibility over millions of bend cycles. Kapton from DuPont is the most recognized brand, but several manufacturers produce equivalent materials.

Polyester (PET) costs less than polyimide but can’t handle soldering temperatures. It’s limited to applications where components attach through pressure-sensitive adhesives or mechanical connectors rather than solder.

For rigid sections in rigid-flex boards, FR4 remains standard. Some high-frequency designs use specialized laminates like Rogers materials, but these add cost and complexity.

Copper Selection: RA vs ED

This is where many designers make their first mistake. There are two types of copper foil used in flex circuits:

Rolled Annealed (RA) copper has elongated grain structure aligned with the rolling direction. This gives it superior fatigue resistance—critical for dynamic flex applications where the circuit bends repeatedly throughout its service life.

Electrodeposited (ED) copper has a columnar grain structure that’s more prone to cracking under repeated flexing. It costs less and works fine for static bend-to-install applications, but specifying ED copper in a dynamic design invites failure.

Copper Type	Grain Structure	Flex Fatigue Resistance	Best Use Case
Rolled Annealed (RA)	Elongated, aligned	Excellent	Dynamic flex applications
Electrodeposited (ED)	Columnar	Good for static only	Bend-to-install designs

Adhesive vs Adhesiveless Construction

Traditional flex laminates bond copper to polyimide using acrylic or epoxy adhesives. Adhesiveless constructions eliminate this layer, resulting in thinner overall thickness and better bend performance. For dynamic applications or designs requiring tight bend radii, adhesiveless materials are worth the cost premium.

Coverlay and Flexible Solder Mask

Coverlay is a polyimide film with adhesive backing that protects flex circuits. Unlike rigid board solder mask, coverlay must be mechanically punched or laser-cut with windows for pad access before lamination. This requires planning coverlay openings during design—you can’t simply define them in Gerber data like solder mask.

Flexible solder mask (also called photoimageable coverlay) applies like liquid solder mask but remains flexible after curing. It’s easier to process than film coverlay but has thickness limitations and different electrical properties.

Bend Radius Calculation: The Foundation of Flex PCB Design

Nothing kills flex circuits faster than exceeding their bend radius limits. The math isn’t complicated, but understanding when and how to apply it prevents the cracked traces that cause field failures.

Static vs Dynamic Flex Applications

Static flex (also called “bend-to-install” or “Use A” per IPC-2223) refers to circuits that bend during assembly but remain fixed in the final product. Examples include folding a flex cable into position inside a laptop or bending a circuit to fit a curved enclosure.

Dynamic flex (“Use B”) describes circuits that bend repeatedly during normal operation. Think of the flex cable connecting a printer head, a laptop hinge, or the folding mechanism in a foldable smartphone.

The distinction matters enormously for design rules. Dynamic applications need much larger bend radii and more conservative trace routing to survive millions of flex cycles.

IPC-2223 Bend Radius Guidelines

The IPC-2223 standard provides minimum bend radius ratios based on circuit construction and application type:

Construction	Static Flex (r/h ratio)	Dynamic Flex (r/h ratio)
Single Layer	6:1	100:1
Double Layer	12:1	150:1
Multilayer	24:1	200:1+

Where r is the minimum bend radius and h is the total thickness of the flexible portion.

Bend Radius Calculation Example

Let’s calculate the minimum bend radius for a double-layer dynamic flex circuit with a total thickness of 0.2mm:

Minimum bend radius = (r/h ratio) × thickness Minimum bend radius = 150 × 0.2mm = 30mm

For a static application with the same construction: Minimum bend radius = 12 × 0.2mm = 2.4mm

This illustrates why understanding your application is critical—the dynamic requirement is over 12 times more demanding.

Practical Bend Radius Tips

From experience, I recommend adding margin to calculated minimums:

• Add 20-30% to calculated values for production variation
• Measure bend radius from the inside surface of the bend, not centerline
• Account for any stiffeners or component mounting near bend zones
• Test prototypes at tighter radii than production to validate margin

Trace Routing Best Practices for Flex Circuit Design

Trace routing in flex circuits follows different rules than rigid boards. The copper must survive repeated stress without cracking, which changes how you approach layout.

Perpendicular Trace Orientation

Route traces perpendicular to the bend axis whenever possible. Traces running parallel to the bend experience alternating tension and compression with each flex cycle, accelerating fatigue failure. Perpendicular traces flex more evenly and last longer.

When you must route parallel to the bend, use curved transitions rather than running traces straight into the bend zone.

Avoid Sharp Angles

Sharp 90-degree corners and acute angles create stress concentration points where cracks initiate. Use curved traces with the largest radius your design allows. If you need direction changes in the bend zone, use 45-degree angles or smooth arcs rather than right angles.

I-Beaming Prevention

I-beaming occurs when traces on opposite layers of a double-sided flex align directly over each other, creating a stiff beam that resists bending. The flex naturally wants to bend around this stiff section, concentrating stress at the edges.

Stagger traces on opposite layers so they don’t overlap in bend zones. This distributes stress more evenly across the cross-section and allows smoother flexing.

Read more different PCB Design services:

Trace Width Considerations

Wider traces resist cracking better than narrow traces, but they also reduce flexibility. In bend zones:

• Use the widest traces your routing density allows
• Taper traces gradually rather than making abrupt width changes
• Consider hatched (cross-hatched) traces for power and ground that maintain conductivity while improving flexibility

Teardrop Connections

Add teardrops where traces connect to pads and vias. This gradual transition reduces stress concentration at the pad-to-trace interface. Most PCB design software includes teardrop generation tools—use them.

Via and PTH Placement in Flexible Circuits

Vias create particular challenges in flex circuits. The plated barrel that creates electrical connectivity between layers also creates a rigid structure that can crack under flexing.

Keep Vias Out of Bend Zones

This is the most important via rule: never place vias in areas that will bend. The rigid via barrel can’t flex with the surrounding material, so stress concentrates at the via edges until the barrel cracks.

Place vias at least 20 mils (0.5mm) away from bend zones. If your design absolutely requires vias near bends, move them onto stiffeners where they’re mechanically supported.

Via Reinforcement Techniques

For vias that must be placed in flexible areas (even static flex):

• Add anchors/spurs: Extend short copper tabs from via pads, encapsulated by coverlay, to prevent pad lifting
• Use teardrops: Gradually transition from trace to via pad
• Maximize annular ring: Use at least 8 mils (0.2mm) annular ring—larger if space allows
• Consider anchoring copper shapes: Add copper features around vias that get covered by coverlay for mechanical support

Via-in-Pad Considerations

Unlike rigid boards, flex circuits cannot use resin-filled via-in-pad. The via barrel remains open, which causes solder wicking during assembly—solder flows down through the via instead of forming a proper joint.

If component density demands via-in-pad, either:

• Move the via away from the pad with a short trace
• Use the rigid section of a rigid-flex design for these components
• Specify selective via filling (expensive)

Rigid-Flex PCB Design Considerations

Rigid flex PCB design adds complexity but offers significant advantages for three-dimensional assemblies. The rigid sections support components while flexible sections enable folding, bending, and dynamic movement.

Stack-Up Design for Rigid-Flex

The layer structure differs between rigid and flex regions of the same board. Key principles:

Place flex layers in the stack-up center. This protects flexible materials during outer-layer processing and places flex layers near the neutral bend axis where stress is lowest.

Use even layer counts. Asymmetric constructions warp during lamination and create uneven stress distribution.

Maintain continuous flex layers. The flexible layers run continuously through the rigid sections—they’re not separate boards connected together.

Specify no-flow prepreg for rigid regions. Standard prepreg can flow onto flex areas during lamination, stiffening sections that need to remain flexible.

Transition Zone Management

The boundary between rigid and flex sections requires careful attention. This transition zone experiences stress concentration as the stiff rigid section meets the flexible ribbon.

Keep components, traces, and vias away from transitions. Maintain at least 50-60 mils (1.27-1.52mm) clearance from the rigid-to-flex boundary.

Avoid sharp corners in the flex outline near transitions. Use radii at corners to prevent tear initiation.

Consider transition zone stiffeners that taper gradually rather than ending abruptly.

Bookbinder Construction for Sharp Bends

When designs require bend radii tighter than standard formulas allow, the bookbinder technique uses progressively longer flex layers. Like pages in a book spine, each layer extends slightly more than the one beneath it, allowing tight bends without overstressing any single layer.

This technique adds manufacturing complexity and cost but enables bend radius to thickness ratios below 6:1 when necessary.

Stiffeners and Mechanical Support

Stiffeners add rigidity to specific areas of a flex circuit, supporting components, enabling ZIF connector insertion, or reinforcing attachment points.

Common Stiffener Materials

Material	Typical Thickness	Best Applications
FR4	0.2mm – 1.6mm	General component support
Polyimide	0.05mm – 0.3mm	Thickness-sensitive areas
Stainless Steel	0.1mm – 0.3mm	EMI shielding, high heat
Aluminum	0.2mm – 0.5mm	Heat spreading

Stiffener Placement Guidelines

• Position stiffeners to support component weight and assembly forces
• Extend stiffeners at least 1mm beyond the area needing support
• Avoid placing stiffener edges directly adjacent to bend zones—vias and traces near stiffener edges are prone to cracking
• Consider thermal requirements when selecting stiffener material

ZIF Connector Reinforcement

Zero-insertion-force (ZIF) connectors are standard flex circuit terminations. The exposed contacts require stiffener backing for proper insertion and latching force distribution. Specify stiffener material and thickness appropriate for your connector’s requirements.

Design for Manufacturability (DFM) Guidelines

A manufacturable design gets built right the first time. These guidelines come from lessons learned working with flex fabricators over many projects.

Critical Dimensions Summary

Parameter	Minimum Recommended	Notes
Trace width	3 mils (0.075mm)	4+ mils preferred for flex zones
Trace spacing	3 mils (0.075mm)	Increase in flex zones
Drill to copper	8 mils (0.2mm)	Critical for flex material movement
Via to board edge	20 mils (0.5mm)	More for flex regions
Annular ring	8 mils (0.2mm)	Larger improves reliability
Coverlay opening	0.2mm from pad edge	Prevents pad lifting
Pad to trace spacing	0.5mm	Required for coverlay windows

Panelization Considerations

Flex circuits are processed in panels, and how your design fits on the panel affects cost. Work with your fabricator early to optimize panel utilization.

Add handling features like tooling holes and fiducials in the panel border areas.

Define breakaway tabs carefully—insufficient tabs cause handling damage while excessive tabs complicate assembly.

Documentation Requirements

Flex and rigid-flex boards need more documentation than rigid boards:

• Bending requirements: Specify minimum bend radius, bend angle, and whether application is static or dynamic
• Stack-up drawing: Show rigid and flex regions with layer materials and thicknesses
• Stiffener details: Material, thickness, location, and attachment method
• Coverlay requirements: Material type and opening tolerances
• Controlled impedance: Specify targets and measurement locations if required

Common Flex PCB Design Mistakes and How to Avoid Them

I’ve seen these mistakes repeatedly across projects. Learning from others’ failures saves time and money.

Mistake 1: Undersized Bend Radius

The Problem: Specifying bend radius too tight for the circuit construction, leading to copper cracking during assembly or field use.

The Fix: Calculate bend radius using IPC-2223 guidelines for your specific layer count and application (static vs dynamic). Add 20-30% margin. Validate with bend testing on prototypes.

Mistake 2: Vias in Bend Zones

The Problem: Placing vias where the circuit needs to flex, causing barrel cracking and open circuits.

The Fix: Map out bend zones early in design and enforce via exclusion in these areas. Move vias to stiffened areas or rigid sections of rigid-flex designs.

Mistake 3: Wrong Copper Type

The Problem: Specifying electrodeposited copper for dynamic flex applications, resulting in premature fatigue failure.

The Fix: Always specify rolled annealed (RA) copper for dynamic flex. For static applications, ED copper can work but RA is safer.

Mistake 4: I-Beaming in Multilayer Flex

The Problem: Aligning traces on opposite layers directly over each other, creating stiff beams that cause stress concentration.

The Fix: Stagger traces on different layers so they don’t overlap in bend zones. Use hatched ground planes instead of solid copper.

Mistake 5: Sharp Trace Angles

The Problem: Using 90-degree corners and sharp direction changes that create stress concentration points.

The Fix: Use curved traces and 45-degree angles throughout flex regions. Enable teardrop generation for pad connections.

Mistake 6: Insufficient Drill-to-Copper Clearance

The Problem: Specifying drill-to-copper distances appropriate for rigid boards but insufficient for flex material movement during processing.

The Fix: Maintain minimum 8 mils drill-to-copper clearance. Increase this for designs with tight tolerances or high reliability requirements.

Mistake 7: Poor Rigid-Flex Transition Design

The Problem: Placing features too close to rigid-flex boundaries, leading to stress concentration and failures at transitions.

The Fix: Keep all copper features, vias, and components at least 50 mils from rigid-to-flex transitions. Use corner radii on flex outlines near transitions.

IPC Standards Reference for Flex PCB Design

Designing to IPC standards ensures manufacturability and provides a common language between designers and fabricators.

Standard	Coverage	Key Contents
IPC-2223	Design guidelines	Bend radius, materials, construction methods
IPC-6013	Performance specification	Quality and reliability requirements
IPC-A-600	Acceptability criteria	Visual inspection standards
IPC-2221	Generic PCB design	Base requirements for all PCB types
IPC-4202/4203/4204	Material specifications	Flex laminate requirements
IPC-TM-650	Test methods	Peel strength, HiPot testing, etc.

Useful Resources for Flex Circuit Designers

Design Tools and Software

• Altium Designer: Full rigid-flex support with 3D visualization and bending simulation
• Cadence OrCAD/Allegro: Comprehensive flex design rules and DRC capabilities
• KiCad: Open-source option with growing flex circuit support

Industry Resources

• IPC Standards: Purchase from IPC (https://www.ipc.org) – IPC-2223 is essential reading
• Flex Circuit Design Guides: Sierra Circuits, Epec, and All Flex publish detailed technical guides
• Manufacturer Design Guidelines: Most flex fabricators provide DFM guidelines specific to their capabilities

Calculators and Tools

• Bend radius calculators: Available from multiple PCB manufacturers
• Impedance calculators: Critical for controlled impedance flex designs
• Stack-up builders: Manufacturer-specific tools help validate constructions

Frequently Asked Questions

What is the difference between flex PCB and rigid-flex PCB?

A flex PCB consists entirely of flexible materials—polyimide substrate with copper conductors and coverlay protection. The entire circuit can bend and flex. A rigid-flex PCB combines rigid FR4 sections with flexible polyimide ribbons in a single integrated assembly. The rigid sections support components and connectors while the flex sections enable bending, folding, and dynamic movement. Rigid-flex eliminates separate boards and connectors, improving reliability and enabling three-dimensional assemblies.

How do I calculate the minimum bend radius for my flex circuit?

Minimum bend radius depends on your circuit construction (layer count) and application type (static vs dynamic). Per IPC-2223, multiply the total flex thickness by the appropriate ratio: for static single-layer flex use 6:1, double-layer use 12:1. For dynamic applications requiring repeated bending, ratios increase significantly—100:1 for single-layer, 150:1 for double-layer, and 200:1+ for multilayer. Always add 20-30% margin to calculated values and validate with bend testing.

Can I place components in the flex area of a rigid-flex PCB?

You can place components on flex areas, but it requires careful design. Use stiffeners to support component weight and provide a solid surface for soldering. Keep components away from areas that will bend during use. For dynamic flex applications, avoid placing any components in bend zones—the rigid component and solder joints can’t survive repeated flexing. SMT components work better than through-hole in flex areas because they don’t create holes that weaken the structure.

Why do flex circuits crack, and how can I prevent it?

Flex circuit cracking typically results from exceeding bend radius limits, fatigue from repeated flexing, or stress concentration at design features. Prevention strategies include: designing adequate bend radius with margin, using rolled annealed copper for dynamic applications, routing traces perpendicular to bend axes, avoiding vias and sharp trace angles in bend zones, staggering traces on opposite layers to prevent I-beaming, and using teardrops at pad connections. Testing prototypes under actual use conditions before production identifies problems early.

What copper type should I specify for a dynamic flex application?

Always specify rolled annealed (RA) copper for dynamic flex applications. RA copper has an elongated grain structure that provides superior fatigue resistance under repeated bending—it can survive millions of flex cycles when designed properly. Electrodeposited (ED) copper has a columnar grain structure that’s more prone to cracking under repeated stress. While ED copper costs less and works acceptably for static bend-to-install applications, using it in dynamic designs significantly increases failure risk.