Construction technology
An external trace of 35 μm copper carrying 3 A with a 10 °C rise needs 1.37 mm of width; on an inner layer, 3.56 mm. Inside the board the heat gets out worse.
01The printed circuit board
The printed circuit board is at once the mechanical support and the wiring of a device. It is made on a laminate: the most common is FR-4, glass-fiber cloth with epoxy resin, which is specified by its glass transition temperature (Tg), its permittivity and its thickness, typically 1.6 mm. For microwaves, PTFE or ceramic laminates are used, with lower losses and more stable permittivity. Copper is specified in ounces per square foot: 1 oz is equivalent to about 35 μm.
A board can have one, two or many layers. In multilayer boards, the inner layers are etched separately and pressed together with sheets of resin (prepreg); the internal power and ground planes give a low-inductance return and shielding. The drawings and the representation standards were covered in computer-aided design environments.
02Manufacturing
| Stage | What is done |
|---|---|
| Drilling | Component holes and vias, with a drill bit or a laser for microvias |
| Plating | Electroless and electrolytic copper on the hole walls |
| Photolithography and etching | A photosensitive film defines the traces and the acid removes the excess copper |
| Solder mask | Lacquer that covers the copper except at the pads; prevents solder bridges |
| Finish | Protects the pads: hot-air solder leveling (HASL), electroless nickel immersion gold (ENIG) or organic coating (OSP) |
| Silkscreen and testing | Component legends and electrical continuity and isolation test |
The manufacturer publishes its design rules: minimum trace width and spacing, minimum drill diameter, annular ring around each hole and distance to the edge. The design is sent to it as Gerber or ODB++ files, with the drill file.
03Trace width
A trace heats up by the Joule effect and the heat has to escape to the air or to the laminate. The IPC-2221 standard gives an empirical relationship between the current, the allowed temperature rise and the cross-section of the trace:
The width required by IPC-2221 as a function of current, for an external layer (blue) and an internal one (purple), with the chosen copper thickness and temperature rise. The panel also gives the resistance and the voltage drop in 10 cm of trace at 20 °C.
04Insulation, impedance and heat
Between conductors at different voltages two distances have to be respected: the clearance (clearance), which prevents arcing, and the creepage distance (creepage), measured along the surface, which prevents conduction through dirt and moisture. Safety standards, such as IEC 62368-1, set them according to the voltage, the pollution degree and the type of insulation; a milled slot in the board lengthens the creepage distance.
In fast signals, the trace and the ground plane form a transmission line —microstrip on outer layers, stripline on inner ones— whose impedance depends on the width, the dielectric thickness and its permittivity; manufacturers control it on request, typically 50 Ω. To remove heat from a component, copper planes and thermal vias are used, which conduct it to the opposite side or to a heat sink.
The equipment ends up in an enclosure, which is specified by its ingress protection rating according to IEC 60529: the first digit indicates the protection against solids, from 0 to 6, and the second against water, from 0 to 8. An IP65 enclosure is dust-tight and withstands water jets.
05In the lab
Pass increasing currents through traces of different widths on a test board and measure their temperature with a thermocouple or a thermal camera; compare with IPC-2221.
Load a manufacturer's rules into the design tool and run the check on a course board.
Calculate the width of a 50 Ω microstrip on 1.6 mm FR-4 and verify it with a reflectometer.
06Common mistakes
- Sizing an internal trace as if it were external. It needs more than double the width for the same heating.
- Ignoring the voltage drop. A trace that does not heat up can still lose tens of millivolts.
- Forgetting creepage distances in the mains area. The safety distances are not those of the board manufacturer.
- Designing without the manufacturer's rules. A spacing that cannot be manufactured is discovered only when ordering the board.
07Self-assessment
What width does IPC-2221 require for 1 A on an external 1 oz layer with a 10 °C rise?
About 0.30 mm, 12 mil.
What happens to the width if 2 oz copper is used?
It is halved: the required cross-section is the same.
What is the difference between clearance and creepage distance?
The first is measured in a straight line through the air; the second, following the surface of the insulator.
What does IP67 indicate?
Dust-tight and protected against temporary immersion in water.
08Further reading
- Clyde F. Coombs and Happy T. Holden (eds.). Printed Circuits Handbook. 7th ed., McGraw-Hill, 2016. The reference on printed circuit materials, manufacturing and design.
- Howard Johnson and Martin Graham. High-Speed Digital Design: A Handbook of Black Magic. Prentice Hall, 1993. Traces as transmission lines and ground planes.
- Eric Bogatin. Signal and Power Integrity — Simplified. 3rd ed., Prentice Hall, 2018. Trace impedance, planes and power distribution.