Estimated reading time: 6 minutes

Fresh PCB Concepts: Managing PCB Trace Width and Spacing

As a fabricator, I know that trace width and spacing are some of the first items reviewed when determining whether a PCB can be manufactured reliably. They may look like simple dimensions in the design data, but the ability to reproduce them consistently depends on several factors, such as the circuit's location, the copper weight used, the design density, and any additional plating requirements. These can all change what is realistically achievable.

One of the most common mistakes is assuming that the same minimum trace and spacing requirements can be applied to every layer of the PCB. Inner and outer layers go through different manufacturing processes, and those processes affect how small the finished features can be.

Inner layer circuitry is generally created by applying an image to the copper foil and etching away the unwanted copper.  This is commonly referred to as a subtractive process because the unwanted copper is subtracted from the panel by etchant. Once the inner layer has been etched and inspected, it is laminated into the finished board.

Outer layers require more processing. In addition to being imaged and etched, they must undergo copper plating to deposit copper inside the drilled holes and form plated through-hole (PTH) connections. During this process, copper is not only deposited inside the holes. It is also added to the surface of the outer layer circuitry. 

This process is commonly considered an additive process because copper is added to the panel. This means the factory must start with an outer layer image that is different from the final desired geometry. The traces and spaces are adjusted or compensated to account for the copper added during plating and later removed during etching. Because of this, a factory may be able to produce smaller trace and spacing values on an inner layer than it can reliably produce on an outer layer when both layers start at the same base copper deposition.

It is also important to understand what the cross-section of an actual copper trace looks like. A trace does not normally have perfectly straight, square walls. During etching, the chemistry removes copper downward, but it also removes some copper from the sides of the trace. In simple terms, the finished trace normally has a slightly tapered trapezoidal shape. It is often narrower at the top and wider where it meets the laminate. The thicker the copper, the farther the etching chemistry must travel to remove the unwanted material. This means the copper is exposed to the etchant longer and more sideways etching can occur. The factory can compensate for this by adjusting the artwork, but there is a practical limit to how much compensation can be made before the traces become difficult to control, or the spaces between them become too small. This is why minimum trace width and spacing must increase as copper weight increases.

Half-ounce and one-ounce copper can generally support finer features than 2- to 4-ounce copper. As the copper gets thicker, the factory needs more room to form the traces and completely remove the unwanted copper from the spaces between them. The challenge is not only maintaining the finished trace width. The factory must also make sure that all the copper between adjacent features is removed.

If the spacing is too small for the copper thickness, some copper may remain at the base of the space (remember the traces are trapezoidal shaped). This can create copper slivers, reduced electrical spacing, or, in the worst case, a short circuit. At the same time, extending the etching process to fully clear a tight space can remove too much copper from the traces themselves. The factory is always balancing the need to fully clear the spaces without reducing the traces below their required finished width.

Designers should also understand the difference between starting copper and finished copper. This is especially important on the outer layers. A board may start with 1-ounce copper foil, but additional copper is added to the surface during hole and pattern plating. The finished copper thickness can therefore be considerably greater than the starting foil.  It is the finished copper thickness that ultimately affects the outer layer trace geometry and available spacing.

These considerations become particularly important in dense areas of the design. A board may have generous trace width and spacing across most of its surface while still containing one or two very difficult locations. The most common examples are the routing channels inside or immediately around a BGA footprint.

BGA areas often require several traces to pass between tightly spaced pads or vias. A small reduction in the available space can determine whether one, two, or even three traces can be routed through a channel.

The most difficult area of the design will normally control the manufacturing capability required for the entire board. A PCB may use 10-mil traces and spaces across 95% of the design, but if it contains 4-mil traces and spaces inside one BGA footprint, it is still a 4-mil design from the factory’s perspective. That one dense area may require a more capable factory.

For this reason, it is generally better not to apply the smallest design rules across the entire PCB unless they are truly needed. Larger features should be used wherever space allows, with tighter rules limited to the areas that require them.

Via treatments can also have a significant impact on outer layer trace width and spacing. This is particularly important when IPC-4761 Type VII filled and capped vias are used. With a Type VII via, the hole is plated, filled, planarized, and then covered with additional copper plating. This process is commonly used for via-in-pad designs because it provides a flat, solderable surface over the filled via.

The important point is that the additional copper cap requires another plating operation. Depending on the factory’s process flow, this can introduce a fourth copper plating process affecting the outer layer surface. Each plating process adds copper not only where it is needed over the filled via, but also to other exposed copper features on the panel.

As more copper is added to the sides and tops of the circuitry, the traces become wider and the spaces between them become smaller. This can create a significant challenge when the design combines Type VII filled and capped vias with fine traces, tight spacing, or dense BGA routing.

A design that may be practical with standard plated through vias will require larger outer layer trace and spacing values once filled and capped vias are introduced. The exact impact will vary by factory. Some factories have specialized equipment and plating methods that give them better control over the amount of copper added during cap plating. Other factories may require more conservative design rules. Type VII via treatment should therefore not be viewed only as a hole requirement. It can affect the manufacturability of the entire outer layer.

Factory design guidelines often list minimum trace width and spacing values, but these values need to be understood in context. A published minimum will only apply to a specific buildup or configuration. It may also represent the factory’s absolute capability rather than a preferred value for stable production.

There is an important difference between what a factory can produce and what should be used for a reliable production design. Designing every feature at the factory’s absolute minimum leaves very little room for normal manufacturing variation. It can reduce yields, increase costs, and make it more difficult to move the product to another approved factory in the future. Whenever possible, the design should include some margin above the stated minimum.

Trace width and spacing should also be reviewed as part of the complete PCB construction rather than as isolated dimensions. The layer location, starting and finished copper thickness, BGA density, via sizes, pad diameters, via treatment, and controlled impedance requirements all work together.

Small design adjustments can have a large effect on manufacturability. Increasing a trace or space by even a small amount may allow the board to be built by a wider group of factories. It may also improve yield, reduce cost, and make the design easier to support throughout its production life. In dense BGA areas, changing the via size, pad diameter, layer assignment, or escape routing strategy may provide enough additional room to avoid pushing the entire design into a more difficult capability level.

There is no single trace and spacing value that is correct for every PCB. The appropriate dimensions depend on the copper thickness, layer location, fabrication process, and overall design density. The best approach is to involve the PCB supplier early, especially when the design includes heavy copper, dense BGA routing, via-in-pad structures, or IPC-4761 Type VII via treatment.

Jeffrey Beauchamp is a field applications engineer with NCAB Group.