Micro PCB Design: Fine Lines and Microvias

Line widths that were once exotic are becoming ordinary. A designer who a few years ago worked with a 75 micrometre minimum — three thousandths of an inch — may now be asked for 30 micrometres or less, which is roughly a thousandth of an inch. Halving or quartering the area of a board is possible at those dimensions, but not with the same design rules: a micro PCB is made by a different and more demanding process, and the rules follow the process.

Why Conventional Processing Stops Working

Standard dry film, standard imaging and standard etching will not produce lines below about 75 micrometres reliably. The resist cannot resolve the feature, the etchant undercuts it, and the result is inconsistent enough to be unusable in production.

Photolithographic imaging is one route to the very fine lines and spaces, and the shops that adopt it gain a real capability difference. Those that do not will find that staying competitive requires them to offer at least 50 micrometre lines and spaces, and eventually 30 micrometres. That is a significant change for shops which today do not routinely offer even 3 thousandths of an inch.

What Is Actually Available

Capability in fine-line work is not uniform, and it helps to know which kind of supplier is being asked for what.

The most capable volume production of fine circuits is concentrated in Asia, where processes were developed specifically for handheld consumer products and deliver lines in the 40 to 50 micrometre band. A second, much smaller group of research-oriented suppliers makes very specialised circuits with features below 40 micrometres on polyimide, but the material is expensive, lead times can run to three months and volumes are low.

A third group consists of mid-sized board manufacturers scaling up quickly: they offer modest production quantities with line widths between 75 and 40 micrometres, delivering thousands of pieces within a few weeks. The fourth group is conventional fine-line production at 125 to 75 micrometres, with high volumes and many participants.

Beyond those, newer processes are now capable of 30 micrometre lines and spaces on ordinary FR-4 as well as on polyimide, which is the capability that changes what a design can look like. As this kind of work spreads, layout engineers will need to become familiar both with the new design rules and with the trade-offs they bring.

Designing for Fine Lines

The first rule is that copper thickness has to come down with line width. A 30 micrometre line cannot be made in one-ounce foil; the aspect ratio of the etched feature would be unmanageable. A useful reference point is that 25 micrometre lines can be produced in 18 micrometre copper, and that is close to the practical ceiling.

Thinner copper is not usually a problem electrically. Unless the design carries high current, a fine trace is perfectly adequate, and where higher current is needed, the solution is to widen the specific conductors that carry it rather than to thicken the whole layer. A 30 micrometre line is mechanically robust, and its exposure to physical damage is largely eliminated by the solder mask that covers it.

Concerns about fragility are also misplaced in context. Designers already work with wire bonds in the 25 to 13 micrometre range connecting a die to its carrier, and fine traces on a board are protected far better than those. Fine features are usually buried on inner layers or covered by mask, which effectively locks them in place, and the adhesion of copper to the board surface has been improved specifically to suit these small geometries.

One convention has turned out to be unnecessary. Early micro designs used generously rounded transitions where a thin trace met its pad, on the assumption that the step would be a weak point. Over time this proved to be surplus: routing the trace directly into the pad is strong and reliable, while the extra fillet increased the image writing time and the cost.

Microvias and Hole Size

Vias have physical limits that traces do not, and they are set by chemistry and by the drilling method.

Below about 50 micrometres, plating chemistry cannot reliably coat the hole wall, and the via quality degrades. Lasers can drill considerably smaller holes than that, down to around 20 micrometres, but a hole that cannot be plated is not useful. Laminate thickness also constrains the minimum via diameter: for plated microvias the aspect ratio limit is about two to one, so a 3 thousandth of an inch microvia is limited to a 6 thousandth of an inch laminate.

Laser drilling has its own depth limit. As diameter shrinks, so does the ability to penetrate the laminate cleanly, and a 3 thousandth via is limited to roughly 4 to 5 thousandths of depth in FR-4, extending to 6 or 7 thousandths in the glass-free laminates used for high density interconnect work.

There is a compensating benefit. Microvias may not go as small as traces, but the annular ring around them becomes much smaller, which recovers a great deal of the area the via would otherwise consume. On an early micro design, a 9 thousandth of an inch pad with a 3 thousandth via was considered tight for conventional fabrication. Precise laser methods allow a 5 thousandth pad with the same 3 thousandth via — a substantial saving across a dense board.

The work involved in making fine vias, and the alternatives used at the extreme end of density, are described in this discussion of padless via high density interconnect.

Where the Density Comes From

The arithmetic is worth setting out, because it explains why the change is worth making.

With 75 micrometre lines and 250 micrometre pads, the achievable pitch is about half a millimetre. Between two adjacent pads there is room for one 75 micrometre trace, and that is close to the limit of what most shops can hold — a demanding specification even before yield is considered.

Using microvia technology with 3 thousandth vias, 5 thousandth pads and 30 micrometre lines and spaces, the same layout can be built at roughly 0.2 millimetre pitch. That is close to a fivefold reduction in occupied area compared with the conventional version. The gain does not require smaller components at all: switching to 30 micrometre lines and the smaller pads that accompany them shrinks the board with the same bill of materials.

Practical Rules for Micro Designs

Match the drilling method to the pad size. Drilled holes wander considerably compared with laser-drilled ones, which is what forces a larger pad-to-hole margin. A drilled hole is normally given a 12 thousandth pad with a 6 thousandth hole, whereas a laser-drilled microvia can use a 5 thousandth pad with a 3 thousandth hole.

Resize everything, not just the traces. Every element of a conventional design needs to be adapted to the smaller dimensions, and this is where experienced layout engineers most often slip. The most common error is a hole that is too large — a habit carried over from conventional work. Oversized holes make a micro design perform below its capability, and in some cases stop it working altogether.

Angle the corners. When routing fine features, use the same techniques as any dense board but favour angled turns over right angles. An angled corner spreads the stress of the turn over a larger area instead of concentrating it at a point.

Choose the supplier as a partner. A micro design depends on a fabricator who can do this work consistently, and that relationship is more valuable than a quotation. A partner who knows the process can tell the designer which features are achievable at each step, which is the difference between a design that is manufacturable and one that is merely drawn. The constraints that govern trace geometry on any board still apply, and the underlying calculations are set out in this note on trace width calculation.

Fine-line capability also changes what the rest of the layout can do with the space it recovers. Reductions in via and pad size feed directly into increased routing density, as covered in this review of HDI layout shrinkage and microvia rules.

FAQ

Why can a 30 micrometre line not be made in one ounce copper? Because the aspect ratio of the etched feature becomes impractical. Thinner copper is required, and a useful reference is that 18 micrometre copper supports lines of about 25 micrometres.

Why can a laser drill smaller holes than can be plated? Because plating chemistry needs access to the hole wall to deposit a continuous layer, and below roughly 50 micrometres it cannot do so reliably. Drilling a hole that cannot be plated produces a via that is unusable regardless of how cleanly it was formed.

Do fine traces need rounded transitions into pads? They do not. Direct routing into the pad is strong and reliable, and the extra fillet adds image writing time and cost for no measurable benefit.