Controlled impedance in flex and rigid-flex printed circuit boards requires balancing electrical performance against physical construction. Trace geometry, dielectric constant, distance to the reference plane, shielding method, copper thickness, and layer count can all affect the finished circuit’s thickness and flexibility.
These relationships matter most when a design combines high-speed signals, EMI or RF shielding, higher current requirements, and limited space. A stack-up that meets the required impedance must also support the application’s mechanical bend requirements.
Why Controlled Impedance Affects Flex Circuit Construction
Controlled impedance supports signal integrity in high-speed flex and rigid-flex PCB designs. Achieving the specified impedance requires control over several related variables:
- Trace width
- Trace-to-ground spacing
- Differential-pair spacing
- Dielectric material properties
- Distance between the signal trace and its reference plane
- Layer arrangement within the stack-up
In standard construction, a core may be 1 mil thick. Controlled impedances commonly require a minimum core thickness of 2 to 4 mils. Increasing the distance between the signal layer and reference plane can help achieve the required impedance, but it also increases the circuit’s overall thickness.
This increase matters in flex and rigid-flex PCB designs because added thickness can reduce flexibility and affect the circuit’s ability to meet the application’s bending and space requirements.
Factors That Determine Trace Impedance
PCB trace impedance is influenced by trace width, dielectric properties, and the distance between the trace and its reference plane. These factors must be evaluated together rather than selected independently.
Higher impedance requirements may require thinner traces, more distance between the signal trace and reference plane, or a combination of both. Increasing that distance generally requires a thicker core.
The dielectric constant of the selected material also influences the required construction. A material with a lower dielectric constant may allow the design to use a thinner core while maintaining the specified impedance. Material selection must therefore account for both electrical performance and mechanical bend requirements.
Designing for 60-Ohm and 120-Ohm Impedance Requirements
Note that 60-ohm single-ended signals and 120-ohm differential signals are higher-end controlled impedance requirements that may require thicker cores.
For these designs, trace width, differential-pair spacing, dielectric constant, and distance to the reference plane must be coordinated carefully. Narrower traces or increased separation from the reference plane may help achieve the specified impedance, but these adjustments affect manufacturability, stack-up thickness, and flexibility.
An example of a signal layer of an impedance design. The white lines are the highlighted impedance lines in the layer.
Specific impedance values should be modeled within the proposed stack-up rather than treated as isolated trace dimensions. The layer construction and selected materials determine which trace geometry can produce the required electrical result.
Stack-Up Planning for Controlled Impedance
Stack-up development establishes the number of layers, their arrangement, and the core and prepreg materials used in the circuit. Controlled impedance requirements must be considered during this stage because the location of signal layers and reference planes directly affects the available construction.
Simulation tools can be used to model potential stack-ups and evaluate how design changes affect impedance.
Variables may include:
- Signal-layer placement
- Reference-plane location
- Core and prepreg thickness
- Dielectric constant
- Trace width
- Differential-pair spacing
- Copper thickness
The design must also leave sufficient space for routing. Advanced impedance requirements may call for precise trace widths and differential-pair spacing, while the available PCB area and overall circuit complexity may limit the routing options.
Trace path and length can also affect signal performance. These routing considerations must be evaluated within the complete stack-up and available board geometry.
Surface Microstrip Construction
A surface microstrip configuration uses an external signal layer and a solid ground reference plane. This is a standard approach for common requirements such as:
- 100-ohm differential signals
- 50-ohm single-ended signals
Stack-up example of a 100-ohm surface micro-strip differential pair.
This construction uses fewer layers than stripline and can help limit overall circuit thickness. However, the exposed position of the signal layer provides a different shielding arrangement than a signal layer located between two reference planes.
Stripline Construction
A stripline configuration places the signal layer between two reference planes. This arrangement provides shielding around the signal traces and may be selected when EMI or RF requirements must be addressed along with controlled impedance.
The additional reference plane and associated core construction increase circuit thickness. Stripline can increase PCB thickness by approximately 60% to 67%.
That increase may affect the circuit’s flexibility. The shielding benefit must therefore be weighed against the mechanical requirements of the flex or rigid-flex circuit board application.
Selecting a Shielding Method
The appropriate shielding approach depends on whether the design requires controlled impedance, noise protection, or both.
Example of a rigid-flex circuit board with shielding.
EMI Shielding Films
EMI shielding films are laminated to the circuit’s external surface. These films are a preferred option when signal noise is a concern, but controlled impedance is not a priority.
This approach provides shielding without significantly increasing the circuit’s thickness.
Copper Shield Layers
Copper shield layers may be required when shielding and controlled impedance must be addressed within the same design. Adding copper shield layers can increase PCB thickness by approximately 50%.
While this construction supports impedance-controlled designs, the added thickness may reduce flexibility and affect the circuit’s bend performance.
Silver Ink Shield Layers
Silver ink shielding is an older technology that has been phased out of many PCB manufacturing locations. It is largely not recommended for controlled impedance applications.
Shielding selection should therefore be based on the electrical requirements and the effect that each construction has on thickness and flexibility.
How Controlled Impedance Interacts with Crosstalk and Attenuation
As signal speeds increase, crosstalk and signal attenuation become greater design concerns. Trace separation can reduce interference between neighboring high-speed signals, but increasing separation also consumes routing space.
Thicker cores provide additional room for trace separation. However, core thickness primarily changes the distance between a signal layer and its reference plane. Lateral spacing between traces remains a routing and layout decision.
For densely routed designs, impedance requirements, trace-to-trace spacing, and available areas must be considered together. Increasing one form of separation may resolve an electrical constraint while creating a space or flexibility constraint elsewhere in the design.
Combining Controlled Impedance with Higher Current
A flex or rigid-flex PCB may need to carry higher current while also maintaining controlled impedance. Higher-current requirements may call for wider traces or thicker copper.
When space is limited, increasing trace width may not be practical. In that case, thicker copper can provide additional current-carrying capacity without requiring the same increase in trace width.
Thicker copper also affects the surrounding construction. The adhesive layers must encapsulate and bond the copper traces while maintaining electrical insulation and structural integrity.
A guideline typically used is 1 mil of adhesive for every ounce of copper thickness. This ratio is used to effectively encapsulated circuitry and to follow requirements associated with IPC. Insufficient adhesive thickness may contribute to incomplete bonding, delamination, or electrical shorts.
Because both thicker copper and thicker adhesive add material to the stack-up, higher-current requirements can increase the finished circuit thickness and further affect flexibility.
How Layer Count Affects Thickness and Flexibility
Additional layers provide more routing area when a design must accommodate greater functionality or a higher density of circuits and components. However, every added layer also contributes to overall circuit thickness.
Moving from a two-layer to a three-layer construction can increase thickness by as much as 40%.
This increase can reduce flexibility and affect whether the circuit is suitable for dynamic or space-constrained applications. The required layer count must therefore be balanced against the circuit’s intended mechanical behavior.
Advanced materials or alternative layering techniques may help limit the thickness increase. Any such option must be evaluated within the electrical, mechanical, and manufacturing requirements of the design.
Prototyping and Testing the Impedance-Controlled Design
High-end controlled impedance designs may require prototyping and iterative testing. This process allows the design team to evaluate whether the selected stack-up, materials, and trace geometry provide the required performance before final production.
A prototype can be used to assess the design under the application’s expected operating conditions. If the results do not meet the required performance, the stack-up, trace geometry, materials, or routing can be adjusted.
This step is particularly important when the design combines several constraints, such as:
- Controlled impedance
- High-speed signals
- EMI or RF shielding
- Higher-current conductors
- High layer counts
- Limited overall thickness
- Static or dynamic bending requirements
Each requirement can influence the same physical construction. Prototyping helps determine whether the complete design achieves the intended balance.
Balancing Signal Integrity, Thickness, and Flexibility
Controlled impedance cannot be evaluated separately from the circuit’s mechanical construction. A thicker core may help achieve the required impedance, while a second reference plane may provide additional shielding. Thicker copper may support higher current, and additional layers may create more routing space.
Each change, however, can increase overall thickness and reduce flexibility.
The design process should evaluate these variables as one system:
- Required single-ended or differential impedance
- Signal speed and routing density
- Trace width and spacing
- Dielectric constant
- Distance to the reference plane
- Surface microstrip or stripline construction
- EMI or RF shielding requirements
- Copper and adhesive thickness
- Layer count
- Available space
- Mechanical bend requirements
A successful flex or rigid-flex stack-up achieves the required electrical performance without making the circuit too thick or inflexible for the intended application.
Summary
Controlled impedance in flex and rigid-flex PCBs depends on the coordinated selection of trace geometry, dielectric material, reference-plane spacing, shielding, copper thickness, adhesive thickness, and layer count.
Surface microstrip can support common requirements such as 100-ohm differential and 50-ohm single-ended signals with a relatively simple construction. Stripline places the signal layer between two reference planes to provide additional shielding, but it also increases thickness. Higher-end requirements such as 120-ohm differential and 60-ohm single-ended signals may require different trace geometry and thicker cores.
Current-carrying requirements, shielding layers, and additional circuit layers can increase thickness further. Because those changes may reduce flexibility, controlled impedance calculations and stack-up planning must account for both signal integrity and the application’s mechanical requirements.
Key Takeaways
- Controlled Impedance Requires Thicker Cores and Strategic Stack-Ups: Achieving consistent impedance, especially for 60-ohm single-ended or 120-ohm differential signals, often requires thicker core materials (2–4 mils or more), which increases the overall thickness of the PCB, especially important in high-speed or RF applications.
- Trace Geometry and Dielectric Selection Are Crucial: Impedance is affected by trace width, spacing, and the dielectric constant of the materials used. Thinner cores or low-Dk materials can help reduce thickness while maintaining required impedance values.
- PCB Configuration Impacts Shielding and Signal Integrity: Surface microstrip is common for simple impedance needs, while stripline configurations offer better EMI shielding at the cost of increased thickness. For designs with EMI concerns but no impedance control, shielding films are preferred over copper or silver ink layers.
- Current-Carrying Demands Affect Copper and Adhesive Thickness: Boards that must handle both controlled impedance and higher currents need thicker copper layers. This, in turn, requires proportional adhesive thickness (typically 1 mil of adhesive per ounce of copper) to avoid delamination or electrical issues.
- More Layers = Less Flexibility and More Thickness: As circuit complexity increases, layer counts often go up. This can increase the overall thickness by 40% or more, potentially impacting flexibility. Designers must balance complexity, flexibility, and space constraints when planning high-speed flex or rigid-flex designs.
