Minnitron Ltd

A few pointers for PCB designers – focused on improving manufacturability of circuit boards.

Autorouters are stupid
We see countless circuit board designs which are intended for volume production that have been designed using an autorouter. These circuit boards inevitably have manufacturing problems associated with poor design, which results in a lower yield and subsequently a higher cost per unit and a higher end-product failure rate. We don’t actually charge any extra for manufacturing badly designed boards (although perhaps we should because our yield is effected dramatically) so initially, the designer is unaware of the cost implications. But further along the production line through assembly, testing, shipping and finally use in the field, there will be a noticable increase in product failures and customer returns. Many of which will be attributed to mishandling and/or misuse, but designing a more robust product from the start will allow it to tolerate a greater degree of mishandling and misuse, resulting in fewer customer complaints, and ultimately a lower customer servicing cost.

Autorouters are a quick method for producing small run prototypes, and are generally not a cost effective way to design for volume production. It is possible to improve the manufacturability of autorouted boards by carefully adjusting the design rule settings, and then spending time “cleaning up” after the routing process. But the time this takes is often longer than it would take an experienced designer to achieve a far more superior layout.

Many autorouter designers will set the track and gap settings to the minimum allowable by their PCB manufacturer in order to make the job easier for the autorouter. The autorouter will then happily chug along laying down 6 thou tracks, spaced at 6 thou, regardless of how much room there is on the board.

There may only be a couple of milliamps flowing through these tracks, and 6 thou may be perfectly adequate according to thermodynamic calculations. But it is an extremely delicate track which is very easily damaged with normal handling. Where there is plenty of room on a circuit board, it makes sense to make the tracks much thicker, regardless of the current. Try to aim for 25 thou (0.64mm) track & gap for low current tracks when there is room. Thicker tracks do not cost any extra to manufacture, the only cost is the extra design time for placement, (by an experienced designer - not an autorouter!), but the increased yield will mean the boards are cheaper for us to manufacture (meaning we can continue to keep our prices amongst the lowest in the UK), and the finished product performs better and is more durable and robust.

Are physically more rubust and will withstand all the handling required during pcb manufacture and assembly.
Can withstand higher fault currents for situations that may not have been considered during development.
Have a lower resistance and inductance and therefore a lower voltage drop for the same current – resulting in less electrical noise.
Run at a lower temperature and therefore produce less thermal noise and less physical stress on the pcb substrate, adhesive and copper.
Have a lower thermal resistance, which helps to conduct heat away from “hot-spots”.
Have a higher adhesion strength to the substrate which reduces the chances of track-lifting from mechanical and thermal stress.
Cost the same as thinner tracks to manufacture.

Via Holes
Try to minimize the number of via holes. A PTH circuit board with very few via holes is better than the same circuit board with many via holes for the following reasons:

When deciding on the dimensions for a via hole, it is important to remember that when the board is manufactured the holes are actually drilled about 0.15mm larger than the finished hole size to allow for plating. So make sure the via pad diameter has room for this, and for alignment tolerance. There wants to be at least 0.2mm between the edge of the hole (drilled size) and the edge of the pad, but the more the better if there is room. Generally, a via hole diameter will be 1/3rd of the track width. So for a 50 tho track (1.27mm) a 0.45mm via hole would be suitable, with a 0.82mm minimum pad diameter. If there is room, make it a 0.6mm hole with a 1.2mm pad. Try not to use any plated holes smaller than 0.4mm if possible – we can drill much smaller than this, but as with track widths, there are greater cost implications.

Another point to note: For a standard 1oz copper PCB, the via hole plating thickness will only be ½ oz. The 1/3rd hole to track rule means that the cross sectional area of the copper through the hole is actually half that of the copper (hence the increased resistance and inductance). But the current carrying capacity of the via hole is roughly doubled from the heatsinking effect of the copper pads on either side.

Componet Pads
Copper component pads follow the same rules for minimum hole to pad size as via holes, but there are a few extra considerations:

Mechanical strength. The copper pad is not only the electrical conductor for the component wire/leg, but it is also the physical “anchor” which holds the component to the circuit board. This is obviously more relevant for a pcb mounted transformer as opposed to a small resistor for example. If the component is heavy, it will have a high inertia, and when subjected to physical shock will place large stresses on the copper pads holding it in place, which is transferred through the copper to substrate adhesive into the substrate (usually fibreglass ie FR4). So for heavy components, keep the copper pads as large as possible to increase the surface area of copper to substrate adhesive. Also, if the pcb holes can be made just large enough to allow the component to fit tightly, then this will relieve some of the stresses from the copper pads. Sometimes even relatively small & light PCB mounted components will apply considerable stresses to its copper pads, ie trimmer pots, jack sockets, switches, connectors, IC sockets, unusually tall capacitors etc, and these should have larger pads where possible.
Thermal resistance. Quite often, the component leg acts as a heatsink for the component (rectifier diodes for example) and so a large component pad is often necessary for cooling the component. In fact, some components may not be able to achieve their rated power handling if they are not mounted on a suitably sized pad.
PTH or Single Sided. PTH circuit boards have stronger pads than single sided boards because the plating acts like a rivet holding the front copper pad to the rear pad. They also have a lower thermal resistance because there is double the surface area of copper (obviously).