Many trace width, spacing, and via design rules used in rigid PCB designs also apply to flexible circuits. However, flexible materials, coverlay construction, and flex-specific manufacturing processes introduce additional constraints that designers must account for during layout.
The flexibility of polyimide materials, their larger dimensional tolerances, and the specialized plating processes commonly used in flex circuit manufacturing often require larger clearances and more conservative design practices than those used for rigid circuit boards. Understanding these differences early in the design process can help prevent manufacturability issues and improve production yields.
Why Flex Circuit Design Rules Differ from Rigid PCBs
Flexible circuit materials behave differently from rigid PCB laminates because they do not contain glass reinforcement. As a result, dimensional tolerances are generally larger and become more significant during etching and throughout manufacturing processes involving heat, pressure, and moisture.
These material characteristics influence:
- Trace widths and spacing
- Trace-to-pad clearances
- Via sizes and pad dimensions
- Coverlay registration requirements
- Hole plating processes
The cumulative effect of these variables often requires greater spacing and larger feature sizes than would be acceptable in a rigid PCB design.
Trace Width and Spacing Requirements in Flexible Circuits
For most areas of a flexible circuit design, trace width and spacing requirements are primarily determined by the base copper thickness being specified.
Standard industry guidelines are as follows:
- 1/3 OZ copper: 0.003” trace and space
- 1/2 OZ copper: 0.004” trace and space
- 1 OZ copper: 0.005” trace and space
- 2 OZ copper: 0.007” trace and space
Copper thicknesses greater than 2 OZ are seldom used in flexible circuit designs because they can significantly reduce flexibility and bend capability.
Example of trace to adjacent pad spacing.
Copper Type Also Affects Flex Performance
The copper used in flex circuits differs from that commonly used in rigid PCB construction.
Most flex circuit designs begin with electro-deposited copper that is subsequently processed into rolled annealed copper. This changes the grain structure from a vertical orientation to an elongated horizontal configuration. The resulting material provides greater ductility, making it better suited for applications requiring repeated flexing or enhanced bend reliability.
To preserve these mechanical advantages, many flex circuits avoid additional copper plating on external traces during hole plating operations. In these designs, the base copper remains the finished copper thickness.
Trace-to-Pad Spacing Requirements
Trace spacing requirements become more restrictive when traces pass adjacent to external component pads.
If the adjacent pad is a via pad, the standard trace and spacing rules based on copper thickness generally apply. Additional clearances become necessary when traces are routed near external SMT or PTH pads because material tolerances and coverlay or soldermask requirements must also be considered.
Designs Using Polyimide Coverlay
When polyimide coverlay is used, trace-to-pad spacing should typically be increased to a minimum of 0.010".
This larger clearance helps prevent:
- Exposed traces
- Coverlay encroachment onto pads
- Registration-related manufacturing issues
Coverlay material exhibits similar dimensional tolerances to the flex core itself. Additionally, SMT and PTH openings are mechanically created before the coverlay is aligned and laminated to the circuit surface. These openings can further affect coverlay dimensional stability and increase registration tolerances.
Designs Using Flexible Soldermask
Flexible soldermask requires less spacing than coverlay because no separate coverlay alignment process is involved.
A typical trace-to-pad spacing of approximately 0.006" can be used when flexible soldermask is applied.
Hybrid Coverlay and Soldermask Constructions
Many flexible circuit designs use a combination of coverlay and soldermask on the same layer.
In this approach:
- Soldermask is used in densely populated component areas where tighter spacing is required.
- Coverlay is used throughout the remainder of the circuit to provide protection and durability.
This hybrid approach can help balance manufacturability, spacing requirements, and circuit protection.
Via Hole and Pad Size Requirements
Via sizing in flex circuits is influenced by both material dimensional tolerances and the plating processes used during manufacturing.
Example of via pad size.
Undersized via pads are one of the most common manufacturability issues encountered in flexible circuit designs.
Typical Via Sizes
Because flex circuits are generally thinner than rigid PCBs, smaller via holes can often be used. The thinner construction reduces the hole-depth-to-diameter ratio, making hole plating easier to achieve.
Common via sizes include:
- Mechanically drilled 0.008" hole
- Mechanically drilled 0.006" hole
- Laser-drilled 0.004" hole
Recommended Via Pad Dimensions
For mechanically drilled vias, the recommended pad oversize is:
- Minimum: +0.010"
- Preferred: +0.012" to +0.014"
For example:
- 0.008" drilled hole
- 0.018" pad diameter minimum
The preferred larger pad dimensions help improve manufacturing yields, particularly in larger circuits where material tolerances can accumulate.
For a laser-drilled 0.004" via, the recommended pad oversize is reduced to 0.008". The laser drilling system's optical registration capabilities help compensate for some material variation, allowing for a smaller pad structure.
Understanding the Selective Pad Plating Process
Most flex circuits use a selective pad plating process, also known as button plating. Unlike traditional rigid PCB plating processes, selective pad plating limits copper deposition to:
- The plated hole barrel
- A small copper ring surrounding the hole
Additional copper is not plated across the entire external circuitry surface.
Cross section of a selective pad plated flex circuit.
This approach helps maintain:
- The original base copper thickness
- The benefits of rolled annealed copper
- Circuit flexibility
- Mechanical bend reliability
- Minimum bend radius capability
How Button Plating Works
A photo-imageable mask is applied to the starting copper surface and processed to expose only the plated-hole locations.
The openings created in this masking process are intentionally larger than the hole diameter to accommodate process and material tolerances. As copper plating builds within these openings, a raised copper ring, or button, forms around the hole.
The height of this plated button depends on the circuit layer count and required IPC copper thickness.
For a 2-Layer Design
- Minimum copper plating thickness: 0.0005"
- Typical button height: 0.0007" to 0.0008"
For a Design With 3 Layers or More
- Minimum copper plating thickness: 0.001"
- Typical button height: 0.0012" to 0.0014"
Why Via Pads Must Be Larger in Selective Pad Plating
The raised button structure created during selective pad plating introduces surface topography that directly affects imaging operations.
During circuit imaging, the photo-imageable material must conform over the plated button. Adequate flat pad area is required between the plated button and the pad perimeter to maintain proper adhesion.
This requirement is one reason for the previously specified minimum 0.010" pad-to-hole oversize.
Without sufficient pad area, the photo-imageable material may flake or lose adhesion, significantly reducing manufacturing yields.
Summary
Flexible circuit design rules differ from those used for rigid PCBs because of the materials involved and the manufacturing processes required. While basic trace width and spacing guidelines remain largely dependent on copper thickness, additional considerations such as coverlay registration, trace-to-pad spacing, via pad sizing, and selective pad plating must also be addressed.
Understanding how polyimide materials, rolled annealed copper, coverlay construction, and button plating influence manufacturability helps designers establish layouts that better support production yields, flexibility requirements, and long-term mechanical reliability.
Key Takeaways
- Trace Widths and Spacings Depend on Copper Weight: Flexible PCBs follow similar trace/space rules as rigid PCBs, with minimums ranging from 0.003" (for 1/3 oz copper) to 0.007" (for 2 oz copper). However, heavier copper reduces flexibility and is rarely used beyond 2 oz.
- Coverlay Requires Greater Trace-to-Pad Spacing: When using polyimide coverlay, trace-to-pad spacing must be increased to at least 0.010" to accommodate material tolerances and mechanical punching. Flexible soldermask allows for tighter spacing, around 0.006", and hybrid coverlay/soldermask approaches are often used.
- Via Pads Must Be Oversized to Ensure Yield: Flex circuits demand larger via pads than rigid boards to accommodate button plating and material stretch. A typical 0.008" via hole should have a pad at least 0.018", with +0.012" to +0.014" preferred for volume production.
- Selective Pad Plating Improves Flexibility: The button plating method limits plating to only via barrels and pads, keeping traces at base copper thickness. This enhances flexibility, improves bend reliability, and supports tighter bend radii.
- Laser-Drilled Microvias Allow for Smaller Pads: Laser-drilled vias (as small as 0.004") offer tighter tolerances due to optical alignment, requiring only 0.008" pad oversize. These are ideal for high-density or space-constrained flex designs.
